PRO/ENGINEER 2003年第二季軟體技術文件

 2003/04/01
Be Flexible in Wildfire
Flexible Components is a new function in Pro/ENGINEER Wildfire that gives users added capabilities for assembly management. The Make Flexible command allows users to change solid objects into flexible objects existing in different states inside an assembly. Each occurrence of the component can have a different flexibility assigned to it, and it will only show up as one BOM item. Having this capability eliminates the need for multiple unique object numbers for a single object displayed in different states. Prior to Wildfire, it was necessary to create unique objects or family tables when attempting to display the same spring in different states of compression in the same assembly. This added extra items to the BOM and required a manual change to correct. Figure 1 shows five uncompressed springs assembled to holes in a circular housing. The four springs around the outer surface of the housing are sitting on washers that are located in the middle of each hole.

Figure 1

The center spring is located in a hole that has no washer, so it rests on the surface of the chassis to which the housing is assembled. When the cover of the chassis is installed, the four springs will protrude through the top of the cover while the fifth spring (fully uncompressed) just touches the inside of the top cover. (See Figure 2.)

Figure 2

Compressing the four springs that are assembled to the outer holes on the housing so that they just touch the inside of the top cover, can be accomplished in Wildfire by making the springs "Flexible" components. Highlight one of the springs that you wish to compress and click your right-mouse button. Select Make Flexible from the pop-up menu. (See Figure 3.)

Figure 3

The Varied Items dialog box will appear. (See Figure 4.)

Figure 4

Select the green add button and use the Search Tool to find the dimension in the spring that will allow it to be compressed. Select Apply and select OK from the Select box. The dimension you selected will be visible in the Varied Items box. (See Figure 5.)

Figure 5

Change New Value to allow the spring to just touch the inside of the top cover and select Placement from the Varied Items dialog box. The Component Placement dialog box will appear with a new button called Define Flexibility. This button allows you to go back and modify the flexibility values (varied items) of the spring. Select OK from the Component Placement dialog box to complete the operation. The springs should be completely inside the top cover, as shown in Figure 6.

Figure 6

Inside the model tree, the four springs will have a new icon attached to them indicating that they are flexible components. (See Figure 7.)

Figure 7

--Submitted by Stan Balish, president and chief executive officer, FroTime Inc., San Diego, CA

How to Flatten a Harness Without the Network
(This tip can be applied in Wildfire in the Harness-MFG module.)
In previous releases, harness networks were flattened automatically with the wires, cables or bundles in a flattened harness. The only way to remove the network was to blank on a layer.

In Pro/ENGINEER Wildfire, the config.pro option "fan_with_network" has been added and may be set to NO (default is YES) to exclude the network from being flattened.
--Submitted by Florin Neamtu, principal engineer, PTC technical support, Needham, MA

Determine What Materials to Use
When parts are in the early development stages, it is not always clear which material to use. For example, 50 percent long glass polypropylene has a different performance characteristic and density than 20 percent short glass. Rather than modifying the Pro/ENGINEER part's density every time you want to look at its total weight, you can write a relation to maintain as many options as you wish. See below:

weight_material_1 = density * mp_volume("")
weight_material_2 = density * mp_volume("")

Substitute the material name and density values as needed. The "weight_material_*" parameter then can be displayed as a parametric note on a drawing or used for further calculations.
--Submitted by Steven J. Frey, vice president, Universal Parametrics, Inc., Ann Arbor, MI

Show a Mechanism Position on a Drawing
Under Drag Dialog, snapshot the mechanism position. Use the make-available-in-drawing icon to make the snapshot visible in the drawing. Create a new view or modify an existing view. Set the type as exploded. The mechanism snapshots will be listed as an exploded state.
--Submitted by Ian Turner, design application support, CSC, MBDA UK Account, Stevenage, UK

Drawing Snap Lines
Use snap lines to expedite drawing cleaning. A snap line is a line that shows up on the screen but not on the printed drawing. It allows you to line up balloons, notes or any draft entities that can be moved using the normal move command. When an entity is selected and moved near the snap line, it snaps to it. The moved entity will change colors when it is attached to the snap line. By using the snap line, balloons can be lined up perfectly straight. The figure below shows several balloons lined up on two snap lines.

Snap lines can be defined on individual drawings to locate dimensions, notes, geometric tolerances, symbols and surface finishes. The system positions the snap lines relative to the view outline, a selected model edge or datum plane. After you place an item on a snap line, the item moves if the grid line moves (such as when the view outline expands).
When placing and locating items on snap lines, keep the following two points in mind:

1. When you move an item onto one snap line, its color changes to magenta. If you set the location by pressing the left-mouse button, the item snaps to the snap line. Until you move the item again, the snap line determines its location.
2. If you move an item onto the intersection of two snap lines, the system highlights one of the lines in red. If it snaps that item to more than one set of snap lines at that location, you can navigate all possible sets using the SEL SNAP LINE menu. When you choose Accept, the system locates the item on the intersection of the two snap lines. When you move either snap line, the item moves with it.

To Create a Snap Line:

1. Select Insert >Snap Line on the menu bar.
2. On the Menu Manager, do one of the following:

You can snap an item to one snap line or to the intersection of two snap lines. You can also attach clipped detail entities such as dimensions, witness line endpoints, set datum endpoints and axis endpoints.

You can place the following items on snap lines:

--Submitted by Sayeeprasad G., engineering assistant, Miller Fluid Heads, Artarmon, Australia

Automating Pro/E, Pro/INTRALINK Installation
Here is a not-so-well-documented technique that enables you to:

This will save a lot of time and prevent you from having to be at the computer to make the right picks. Here are the details:

There also is the option of running setup without displaying on screen (use -nographics option): ptcsetup -nographics -uitrail setup.txt.
See the PTC description in TPI 103331 for more information.
This technique is especially useful for installing Pro/INTRALINK. You could incorporate it into your standard installation procedure so all new clients are set up with the correct paths, servers, etc.
--Submitted by Edwin Muirhead, CAD systems administrator, Aberdeen, Scotland, UK and www.geocities.com/proehelp/index.html?admin.htm#setup

Response Pro/Clues 3 - Vol. 2, Issue 3
I would still have to be at the computer to log into it as an administrator and to start the process. A user does not have rights to install most programs. How can I get around this?
--Stephen Galayda, CAD system administrator assistant, HydraForce, Inc., Lincolnshire, IL

Sizing Pro/INTRALINK Columns
To get your Pro/INTRALINK columns to be only as big as needed, point your mouse over the column heading and hit the right-mouse button. They will adjust automatically, usually narrowing to the longest entry listed.
--Submitted by Sandy Buerkle, designer, Welch Allyn Inc., Skaneateles Falls, NY

Response PRO/CLUES 4 - Vol. 2, Issue 3
In addition to resizing one column with a right-click:

--Ed Muirhead, CAD systems administrator, Aberdeen, Scotland, UK.

2003/04/18

Q1- Vol. III, Issue 13
I am trying to model the shin guards (shown below) in Pro/ENGINEER, but I am having trouble getting the shape to be correct. Can you recommend any advanced tutorials or other training guides to help me solve this modeling problem?
--Andrew Walter, engineering student, Australian National University, Canberra, ACT Australia

A1.1- Vol. III, Issue 13
The profile of the skin guard you show on the picture seems quite complex. It is better to first digitize it using a laser digitizer or CMM. Afterward, bring the digitized data into Pro/E.
--Yasir Arfeen, CAD/CAM engineer, OJ Pvt. Ltd., Karachi, Pakistan

A1.2- Vol. III, Issue 13
The best tutorials at student rates can be found at www.frotime.com.
--G. Alexander Korentis, mechanical/biomedical engineer, QCI Engineering, University of Connecticut, biomedical engineering doctoral student, Storrs, CT

A1.3- Vol. III, Issue 13
Take the "Advanced Surfacing Training" course offered by PTC or Rand.
--Chris Boyer, manager of product creation, Freudenberg Household Products LP, Northlake, IL

A1.4- Vol. III, Issue 13
You might try looking into medical archives. If an FTP site exists for your software, you may find proven applications there.
--Craig D. Skogerson, Indio, CA

Q2- Vol. III, Issue 13
I just received Pro/ENGINEER Wildfire and I am concerned about its stability. In the past, I have heard it was wise to wait a few months before installing new versions. Has anyone had problems with Wildfire and would you recommend I wait until any possible bugs are worked out?
--Pascal Normand, designer, research and development, Industrial Handling Division, IPL Inc., St-Damien, Quebec, Canada

A2.1- Vol. III, Issue 13
I've been using Wildfire for about a month and I have not come across any bugs yet. I do stress yet. I have found it much better and easier to use than R2001 once you get to know where everything is. An important addition is the Menu Mapper under the Help menu. To find out how to do something in Wildfire, open the Menu Mapper. The Menu Mapper shows an R2001 screen with the old-style menu layout. After you run through the R2001 way of executing the command, using the R2001 menus shown, the Menu Mapper will show you how to do it in Wildfire. It is an excellent tool.
--Jeff Taylor, mechanical production engineer, Imagination Technologies Ltd., London, UK

A2.2- Vol. III, Issue 13
I installed Wildfire and just did my first real rush job with it. I took nine hours nonstop and a large thermos of coffee. But I got it done. This was the first time I used it. I have had no training on it. That speaks to its usability and the fact that the interface has not changed a lot from the previous version. However, Wildfire crashed four times doing routine tasks. Thankfully, no critical steps were lost, and I was able to carry on. But it is definitely not yet stable.
--Christopher J. Purcell, defense research and development, Canada Atlantic, Dartmouth NS, Canada

A2.3- Vol. III, Issue 13
Wildfire does not work with Pro/INTRALINK.
--Tom Hargrove, fusion energy division, Oak Ridge National Laboratory, Oak Ridge, TN

A2.4- Vol. III, Issue 13
You are right. Often it is better to wait for some builds after the first production edition of a new Pro/E release. I have not tried Wildfire yet, but I'll wait at least a couple of months before using it in a production environment.
--Luca Armellin, mechanical engineer, Metelli SpA, Brescia, Italy

More Answers to Previous Questions
Q1- Vol. III, Issue 12
I have modeled a rod with two bends on two different planes. How do I unbend the rod shown in the image below?
--Herb Spaulding, product engineer, Miller Industries, Ooltewah, TN

A1.1- Vol. III, Issue 12
Create a datum curve that follows the path you want. If it is a 2D path you want to follow, you have to use the 2 Projections option in the Curve menu. Select Insert >Datum >Curve and choose 2 Projections. If you choose two datums at right angles to each other, they will create a datum curve where the two intersect. You can then create a sweep. Select Create >Protrusion >Sweep and choose Select Traj. Select the datum curve you have just selected and sketch a round section. This technique can also be used to create sweeped pipes in assemblies.
--Brian Middlemore, CAD support engineer, NCR Ltd., Dundee, Tayside, Scotland

Bar

Datum curve

A1.2- Vol. III, Issue 12
If you have modeled the rod with a toroidal bend tweak and you want to obtain a straight workpiece, suppress the toroidal features.
--Zachary Popov, mechanical engineer, Technical University, Varna, Bulgaria

Q2- Vol. III, Issue 12
As of Pro/WILDFIRE, the internal datum plane, aka "on-the-fly" created datum plane, functionality is removed. I am wondering if this will impair model building?
--Alexander Fabre, B. Sc. M. E., Avalon Technology Stockholm AB, Sweden

A2.1- Vol. III, Issue 12
This functionality resides within the feature creation. While creating the feature, click on the pause button at the bottom right of the screen. (It is next to the preview button.) Create the necessary axes, planes, points etc, and click on the pause button to continue building the feature. (Planes, axes, points, etc. on the "fly").
--Roman Panov, MCAD application specialist, Engineering Data Resources AS, Norway

A2.2- Vol. III, Issue 12
The "Make Datum" command is not necessarily removed, it has been restructured. An "on-the-fly" datum still can be created by means of the same menu option for creating a datum. The difference in Wildfire is that the "on-the-fly" datum plane is an actual feature in the Model Tree and can be selected for reference when creating other features. So "on-the-fly" datums are now more useful. The only impairment is that users accustomed to the old menu selection have to learn Wildfire's dashboard-style menu structure, which is easy to learn.
--Wes Gerber, mechanical design engineer, ITT Industries, Aerospace/Communications Division, Fort Wayne, IN

A2.3- Vol. III, Issue 12
The internal datum plane functionality is not removed. It is accessed differently. If you wish to create a datum on the fly, use the same icons or menu picks as you would when creating "visible" datums. Datums created during feature creation are listed in the model tree, but are automatically hidden and grouped with the feature being created. In most cases the feature you are creating - such as an extruded protrusion - will grab the plane you create and use it for the sketching plane. If Wildfire does not select the created plane automatically, then you can select it yourself. The important thing to note is that on-the-fly datums are still with us.
--Kellie Wheatcroft, mechanical engineer, Smart Design, Perth, Western Australia

Q1- Vol. III, Issue 12
I have modeled a rod with two bends on two different planes. How do I unbend the rod shown in the image below?
--Herb Spaulding, product engineer, Miller Industries, Ooltewah, TN

A1.1- Vol. III, Issue 12
The model should be recreated with a straight rod and a datum curve defining the shape you want the rod to become and then by using spinal bend. Another option would be to create a sheet metal component of which an edge defines the centerline of the rod. Create a datum curve that is a composite of the edge defining the centerline. Create a solid swept protrusion that follows the curve. Make the sheet metal component small enough to be buried within the rod. Then flat-pattern the sheet metal portion to get your straight rod and suppress to get the bent rod.
--Brian S. Lynn, design drafter/CAD administrator, Weil-McLain, Heating America!, Indiana

A1.2- Vol. III, Issue 12
One way to handle this situation is to create the feature as a datum curve instead of as a solid feature. You can create the path using two datum curves, making sure to make a composite curve afterward. Create an extruded solid the same length as your curves. (See Spinal Before image below.) Create a spinal bend by selecting Feature >Create >Tweak >Spinal Bend. Work your way through the menus and select the extrude material to bend around the composite curve. When asked to select a plane to define the volume of bend, select the opposing end of your extrusion to get the desired result. (See Spinal After image below.) You can create an instance by removing the spinal bend feature giving you both a "bent" and "unbent" form of your part. You can also find an example of this by searching the help files using "spinal" as the keyword.
--Greg Daniel N.D.G.A. systems analyst/MCAD administrator, SPACEHAB, Inc. / Johnson Engineering, Webster, TX

Spinal Before

Spinal After

A1.3- Vol. III, Issue 12
Redefine your trajectory.
--Doug Rogers, project engineer - Fuel Metering Valves, Precision Engine Controls Corp., San Diego, CA

A1.4- Vol. III, Issue 12
If the feature was not created by a trajectory protrusion, create a family table that includes the bent feature. The new instance should have this feature set to No. Include a feature that includes the dimension for the length and modify that number to the correct length when the part is unbent. If it was created by a trajectory protrusion, remodel it or these instructions will not work.
--Karen Thacker, design engineer, Physitron Inc., Huntsville, AL

Q2- Vol. III, Issue 12
As of Pro/WILDFIRE, the "internal datum plane," aka "on the fly created datum plane," functionality is removed. I am wondering if this will impair model building?
--Alexander Fabre, B. Sc. M. E., Avalon Technology Stockholm AB, Sweden

A2.1- Vol. III, Issue 12
I called tech support about this question. They said to just use the Create Datum Icon from the toolbar. It will still be a "datum on the fly". The "Make Datum" menu pick is just not available anymore.
--Greg Morris, associate designer, The Halex Co., Bedford Heights, OH

A2.2- Vol. III, Issue 12
In Wildfire, you can still create datums "on the fly," but when you are finished creating the feature you will have a group in your model tree that contains the feature and the hidden datum planes. You can unhide these datums later and use them for references for other features if you wish.
--Paul Bock, mechanical engineer, Plesh Industries, Inc., Buffalo, NY

A2.3- Vol. III, Issue 12
Based on a recent PTC webcast, the "Datum-on-the-fly" was removed from Wildfire on the assumption that this functionality was mainly used for pattern features-a feature that has been and will continue to be improved with Wildfire.
--Wade Williams, CAD designer, Alfmeier Corp., Greenville, SC

A2.4- Vol. III, Issue 12
The datum "on the fly" method has been removed, but it has been replaced by the ability to create datum features within a command. Once the command has been completed, the feature and the new datum are autogrouped and placed in the model tree. The icon in the model tree looks similar to a copied feature icon.
--Jeff Taylor, mechanical production engineer, Imagination Technologies Ltd., London

Q1- Vol. III, Issue 11
How do I get the measure command to default to "by plane"?
--Bernard Henry, tooling and equipment design engineering, Knowles Electronics, LLC, Elgin, IL

A1.1- Vol. III, Issue 11
I created a mapkey to default to "by plane." It is listed below.
mapkey meas_xyz @MAPKEY_NAMEmeasure_using_xyz;@MAPKEY_LABELmeasure_xyz;\
mapkey(continued) ~ Activate `main_dlg_cur` `ProCmdDToolsMeasure.view`;\
mapkey(continued) ~ Open `measure` `MsrTypeOptions`;~ Close `measure` `MsrTypeOptions`;\
mapkey(continued) ~ Select `measure` `MsrTypeOptions`1 `Distance`;\
mapkey(continued) ~ Open `measure` `DistToOptions`;~ Close `measure` `DistToOptions`;\
mapkey(continued) ~ Select `measure` `DistToOptions`1 `Plane`;\
mapkey(continued) ~ Open `measure` `DistFromOptions`;~ Close `measure` `DistFromOptions`;\
mapkey(continued) ~ Select `measure` `DistFromOptions`1 `Plane`;
Or you can use this one, which I believe is a standard Pro/E config.
mapkey mp #INFO;#MEASURE;#DISTANCE;#FROM PLANE;
--Arnold Collett, senior mechanical designer, Paragon Technology, Inc., Huntsville, AL

A1.2- Vol. III, Issue 11
I do not know if you can change the default, but you can create a mapkey using the following sequence:

Analysis.....Measure...... Pick Distance as the type, then pick the to and from parameters (in that order) and set them to Plane. Stop the mapkey sequence and save it to the appropriate config.pro. By entering a mapkey, you are instantly ready to pick your planes for measuring.
--Richard Cruz, mechanical engineer, Key Technology, Walla Walla, WA

A1.3- Vol. III, Issue 11
I find it most convenient to place an icon in my tool bar linked to a mapkey. I have one for plane-to-plane, plane-to-axis and axis-to-axis. I measure distances so often that I find this a real timesaver. One click and you are there.
--Dave Miller, design engineer, Commodore Machine Co., Bloomfield, NY

Thanks to our readers, we received more than two dozen answers to this question. To read all of the answers to Q1- Vol. III, Issue 11, click here.

Q2- Vol. III, Issue 11
Is there a way to override dimension text in my drawing, such as a linear dimension in which I want to "lie" to state a different number? I know this is kind of a funny question, but it is available in AutoCAD.
--Peter Zeiss. design engineer/project manager, Transparent Container - Tool Design & Mfg. Berkeley, Berkeley, IL

A2.1- Vol. III, Issue 11
Yes there is. Replace {0:@D} with {0:@o}. It will only work if you add text ({0:@D}54, for example). This only works for dimensions created in the drawing and not for feature-driven dims.
--Thierry Declerck, industrial design engineer, Philips Industrial Activities NV, Philips Sound Solutions, Belgium

A2.2- Vol. III, Issue 11
Yes, there is, but it needs to be accomplished with a created dimension. Create the dimension in the drawing, highlight it, go to Properties (the symbolic display will be @D for the dimension). Change @D to @O (the letter O). Any text you enter after the "O" will appear in place of the dimensional value with the leader lines and dimension arrows.
--Mike Brattoli, senior product design technician, Moen Inc., North Olmsted, OH

A2.3- Vol. III, Issue 11
Although I strongly recommend against doing this, it is possible. Edit the dimension text and put an O in place of the D and type the desired text immediately following the O. We restrict our users from doing this without consulting an administrator to prevent problems down the road in manufacturing and inspecting the parts or assemblies.
--Brian J. Hart, mechanical engineer/Pro/E administrator, Lockheed Martin NE&SS-Archbald, Archbald, PA

Q1- Vol. III, Issue 8
PTC announced it might provide a config.pro option in Wildfire that would allow users to continue to use the Ctrl key and the mouse buttons as done in prior releases. Has anyone been able to determine if this is true, and if so, have you implemented it and used it successfully?
--Mike Brattoli, senior product design technician, Moen Inc., North Olmsted, OH

A1.1- Vol. III, Issue 8
I sincerely hope PTC will give Wildfire users the option of reverting to previous zoom/pan/spin control. In a previous Pro/E Digital Digest, a reader suggested buying a five-button mouse (four-button + scroll-wheel button) and binding one of the new buttons to CTRL. A truly brilliant idea!

Try before you buy a five-button mouse. I found it better to have the two additional buttons under my thumb. The symmetrical mouse, with a button on each side, made it difficult to avoid activating the fifth mouse button while holding in the thumb button and one of the standard three buttons while dragging.

It takes a day or two to get used to it, but I would never go back. I have total control with the mouse and it makes the new controls requiring Shift, Ctrl and differing Pan control between 2D and 3D seem like a giant leap backwards.
--Patrick Morris, product designer/mechanical engineer, Allied Telesyn Research, Christchurch, New Zealand

A1.2- Vol. III, Issue 8
There is no config.pro option available, but you can use the spaceball to act as your mouse. I found the spaceball is more useful than the mouse and ctrl button/ Here is the link to spaceball. www.3dconnection.com
--Raymond Yung, mechanical engineer, Arista Networks, Palo Alto, CA

Q1- Vol. III, Issue 10
If I have completed a U-shaped round tube using the sweep function, how can I create the centerline in the drawing?
--Derek Soon, assistant engineer, design, vehicle construction department, DelGro Engineer Pte Ltd.

A1- Vol. III, Issue 10
Make a datum curve. Select the curve as trajectory when you make the sweep. On the drawing, change the line to a centerline. You have to use Hidden line in the drawing view to see the centerline.
--Johannes Noval, mechanical engineer, Denmark

Q1- Vol. III, Issue 9
What kind of Pro/E experience or training is required to become a Pro/E administrator?
--John Kopacki

A1- Vol. III, Issue 9
You need to take the following training courses:

--Jay Sussman, president, Torgon Industries, San Diego, CA

2003/04/21

Q1- Vol. III, Issue 15
I am trying to find a way to get information turned into parameters from Pro/MANUFACTURING. Do you know how to convert mfg_feat.inf file results "cutting time:" and "z_min:" into a parameter that can be used in Pro/RERPORT?
--Patrick Kimlin, owner, NK Designs Inc., Ann Arbor, MI

A1- Vol. III, Issue 15
I never managed to do this. Instead I exported the manufacturing information to a text file and edited it so that it contained only the relevant and applicable information. This included cutting time, speed, feed, tool, etc. Then I put it on the drawing in the form of a note.
--Steven Hatch, production design engineer, Global Marine Systems Ltd., Chelmsford, England

Q2- Vol. III, Issue 15
How can I update Pro/E Wildfire (code 2002490) from Pro/E 2001 (code 2001440)?
--Nguyen Thai Duong, Victory, Hanoi, Vietnam

A2- Vol. III, Issue 15
A user wanting to upgrade to Pro/E Wildfire has two choices:

1. Load Wildfire, but leave release 2001 on your computer.
2. Uninstall release 2001 and install Wildfire.

In either case, the CD will walk you through the installation process. The only real choices that need to be made involve how the licensing is handled on your computer (locked license vs. floating licenses) and whether you should load Help files.
--Mike Brattoli, senior product design technician, Moen Inc., North Olmsted, Ohio

Q1- Vol. III, Issue 10
If I have completed a U-shaped round tube using the sweep function, how can I create the centerline in the drawing?
--Derek Soon, assistant engineer, design, vehicle construction department, DelGro Engineer Pte Ltd.

A1- Vol. III, Issue 10
Create a curve through the center plane of the U-shaped tube following its trajectory. Change the linetype properties of the curve to a centerline.
--Tony Havern, design engineer, Moffett Engineering Ltd., Dundalk Co., Louth, Ireland

A2- Vol. III, Issue 10
In your model select Create Datum Axis >Through Cylinder. Select the swept extrusion. The axis will be placed at the center of your extrusion and can be used in the drawing.
--Terry Hendrick, tool designer, Means Industries, Inc., One Way Clutch Business Unit, Saginaw, MI

A3- Vol. III, Issue 10
If you create it as a hollow pipe, the centerline will show by default.
--Simon Lewis, mechanical design, Control Techniques, Wales, UK

A4- Vol. III, Issue 10
In the model, sketch a curve and modify its line style and color. Use that curve as the trajectory to create the swept protrusion. If the curves are displayed on the drawing, the centerline will show automatically.
--Jason Shuey, tool designer, Anchor Packaging, Paragould, AR

A5- Vol. III, Issue 10
Use a sketched datum curve to create the sweep path. Use the curve to create the sweep. Modify the curve's line style to be centerline style. Make your drawing and create a section view of the part to see the curve.
--Ryan W. Rush, application engineer, EDS TSG/Engineering Systems, Rochester, NY

A6- Vol. III, Issue 10
Unfortunately, this is not an option in Pro/E but there is a work-around. To dimension the centerline of a bent tube, create a datum curve for the trajectory of the swept feature. Instead of sketching the trajectory in the feature creation, create a datum curve as the trajectory. To do this, click on Select Traj and click the datum curve instead of choosing Sketch Traj. This is easily dimensioned in the drawing.
--Luke Andrew, design engineer, Dutro Co., Logan, UT

A7- Vol. III, Issue 10
I had the same problem creating center points for radius centers on drawings. The only way I was able to do it was by creating a cosmetic sketch in the part model parametrically aligned to the radii centers. The same thing can be accomplished to create a cosmetic sketched line for the centerline.
--Kevin Sullivan, product engineer, Nice Ball Bearings, Kulpsville, PA

A8- Vol. III, Issue 10
Create a datum curve and use it to create the sweep (select sweep). In the drawing, show hidden lines and modify the line to centerline.
--Dave Fischer, senior designer, Hobart Food Equipment Group, Troy, OH

A9- Vol. III, Issue 10
Create a cosmetic feature that references the datum curve that was used for the sweep feature. Create a cosmetic sketch and select Use edge, picking the datum curve as the edge to use. Change the appearance of the cosmetic to be a centerline by picking Geom Tools and Cosm Font. Select the sketch edges and change the style using the dialog box that pops up. Any changes to the curve will follow with the cosmetic. If you add or delete a segment of the original datum curve, you will have to fix the cosmetic manually. If you need to control the location of the cosmetic, set it to a unique layer and set that layer for a particular drawing view only.
--Bill Jensen, senior product designer, Dana Traction Technologies

A10- Vol. III, Issue 10
If you swept the U-shaped protrusion along a previously constructed curve, using it as the center point of your U-shaped sketch, you may show the curve in your drawing. You can hit Use Edge of the curve, relate it to the view and place the curve on a layer and turn it off. Change properties of the curve to "centerline". The sketched entity should behave in the drawing as though it were a part of the solid geometry.
--Deron M. Drach, Whirlpool

A11- Vol. III, Issue 10
Set the line style of the driving curve to be centerline and, in the drawing (in display mode/edge display), set that entity to be 'wireframe' in the views in which you want to see it.
--John Wade, Wade Org., UK

A12- Vol. III, Issue 10
The best solution would be to work inversely. Create a datum curve and run the sweep along the curve. The curve's font can be changed later to centerline font. If the swept feature exists already, you may create a composite curve along the edge of the surface of the feature. If it is a tube with a circular section, the surface will be split and you can use the surface-edge option. After the composite curve is completed, you can create an offset curve from it at the correct distance. Be sure to connect the distance with the tube diameter using correct relations.
--Uriel Avron, chief executive officer, Harmonic Systems (UA) Ltd., Israel

2003/04/23

Customizing the Object New Menu in Pro/INTRALINK
Pro/INTRALINK has the capability to create new objects in your workspace. This method involves using the selection Object >New from within the Workspace browser. The problem is that to use this method, you must scroll through many object types before coming across the Pro/ENGINEER object types. (See Figure 1.) This can be frustrating, but there is a way to solve the problem.

Figure 1

If you have administrator privileges within Pro/INTRALINK, you can send the Pro/ENGINEER object types to the top of this list. Open the administration portion of Pro/INTRALINK by selecting Administration from the main Pro/INTRALINK menu or Intralink >Administration from within either the Commonspace or Workspace browser. Once inside the administration portion of Pro/INTRALINK, expand the Object category to view the available options. Select the Object Types category to view all the defined object types in the database. The system will sort according to the object type description field. To easily find the Pro/ENGINEER object types, sort the Description column. Scroll to find the descriptions that begin with Pro/ENGINEER.
There are a few ways to get the object types to appear at the top of the list. Place a symbol or number in front of the description name. (See Figure 2.)

Figure 2

There are only a few Pro/ENGINEER types you need to put at the top of the list. These are:

Using this technique, you can sort other object types commonly used within your environment. To see what the Object New dialog looks like after the change, select it from within the Workspace browser. The object types should appear at the top of the list. (See Figure 3.)

Figure 3

--Submitted by Eric Horn, FroTime Inc., San Diego, CA

Creating a Four-Sided Box With Flanges on Top
This tip covers a fast way to create a standard four-sided box with flanges on top. Typically, a Pro/E user would start the part in Pro/SHEETMETAL and create each wall and flange separately. To save time, start the part in Pro/SOLIDS and convert the part to Pro/SHEETMETAL. This cuts in half the amount of features it takes to create the box or part. This is important when working with large assemblies because it avoids lengthy regeneration times.

With this method, it takes only five features to create a four-sided box with flanges on top.
--Submitted by Charles Niemotka, Tobyhanna Army Depot Pro User Group, Tobyhanna Army Depot, Tobyhanna, PA

Automating Pro/E, Pro/INTRALINK Installation
Here is a not-so-well-documented technique that enables you to:

This will save a lot of time and prevent you from having to be at the computer to make the right picks. Here are the details:

There also is the option of running setup without displaying on screen (use -nographics option): ptcsetup -nographics -uitrail setup.txt.
See the PTC description in TPI 103331 for more information.
This technique is especially useful for installing Pro/INTRALINK. You could incorporate it into your standard installation procedure so all new clients are set up with the correct paths, servers, etc.
--Submitted by Edwin Muirhead, CAD systems administrator, Aberdeen, Scotland, UK and www.geocities.com/proehelp/index.html?admin.htm#setup

Sizing Pro/INTRALINK Columns
To get your Pro/INTRALINK columns to be only as big as needed, point your mouse over the column heading and hit the right-mouse button. They will adjust automatically, usually narrowing to the longest entry listed.
--Submitted by Sandy Buerkle, designer, Welch Allyn Inc., Skaneateles Falls, NY

Recreating Assemblies in Pro/MECHANISM Design
Although it is possible to convert existing assemblies into Pro/MECHANISM, experience shows it is easier to recreate an assembly. One reason is that components often are assembled in a different order than what is required within Pro/MECHANISM.

Avoid conflicts between joint-axis settings and drivers. If joint-axis settings and drivers conflict, the assembly may fail when running the motion. In most cases, the failure is caused by the driving trying to push a component beyond its joint-axis limits.
--Submitted by Ian Turner, design application support, CSC , MBDA UK Account, Stevenage, UK

2003/04/28

Q1- Vol. III, Issue 16
Is there a way to cross-hatch (Xhatch) a section in which the hatching is something other than lines? I would like to have circles or other shapes repeated in my cross-hatching.
--Dan Bailey, product development engineer, Emerson Appliance Motors, St. Louis, MO

A1.1- Vol. III, Issue 16
I can provide a partial answer to your question. To generate cross-hatching other than the default "slanted lines", do the following in Pro/E 2000i^2:

The portion of your question left unanswered is where to find, or how to generate other varieties of cross-hatch patterns to store in this or another working directory. Perhaps others can answer this part or provide a better solution.
--Richard Cruz, mechanical engineer, project engineering, Key Technology, Inc., Walla Walla, WA

Q2- Vol. III, Issue 16
I just received Pro/E2001 and I am trying to create dimensions. It does not work when I place my new dimensions in Sketcher or on the print itself. Is there a special setting that I need to know about?
--Sue Coupal, drafter II, Eaton Corp., Selma, NC

A2.1- Vol. III, Issue 16
Your question is somewhat confusing. If you create a drawing and choose View >Show and Erase, a window will open that gives you the option to pick different types of dimensioning schemes. This function uses the dimensions that you use in Sketcher when creating geometry.
--Garry Enyart, Fort Recovery Industries

2003/05/02

Q1- Vol. III, Issue 17
How do you organize Pro/ENGINEER files? In other words, which EDM/PDM system do you use?
--Dirk Scherer, PROCAD GmbH & Co. KG , Projektleiter, Germany

A1.1- Vol. III, Issue 17
We use MatrixOne as our PDM solution. The MXPRO integration adds a pull-down menu directly in Pro/E and is easy to use for file management and vaulting.
--Emmanuel Stathopoulos, senior mechanical engineer, Hyperchip Inc.

A1.2- Vol. III, Issue 17
We use Product Center from STI/WTC.
--Brian S. Lynn, CAD administrator/design drafter, Weil-McLain, Michigan City, IN

Q1- Vol. III, Issue 16
Is there a way to cross-hatch (Xhatch) a section in which the hatching is something other than lines? I would like to have circles or other shapes repeated in my cross-hatching.
--Dan Bailey, product development engineer, Emerson Appliance Motors, St. Louis, MO

A2- Vol. III, Issue 16
I do not know how to add circles as part of the pattern. You can however create additional cross sections. Go to MOD XHATCH and retrieve one of the existing patterns. You can add/delete lines as well as modify the font and weight. When you finish, select Save, type the name of the pattern and hit Enter. The pattern will be saved in your working directory. After saving it, you can move it to the crosshatching directory. If you want to keep your custom patterns separate from the defaults, create a new folder and add the following line to your configuration file: pro_crosshatch_dir path. You can also assign crosshatch patterns automatically to a cross section. In your part, assign a material by selecting Set Up >Material >Define or Assign. (We utilize a material library). Name your crosshatch files to correspond with the material names. If the system finds a pattern with the same name as the material (without the .xch extension), it automatically assigns it to the cross-hatch section.
--Randy Hagen, sustaining engineer, VIASYS Healthcare, Palm Springs, CA

2003/05/09

Q1- Vol. III, Issue 18
Can anyone explain to me why curves created between two points using the "thru points" option are not accepted as trajectory during sweep feature creation? How can I get around this?
--Manohar Dapakara, Eicher Motors Ltd., Indore, India

A1.1- Vol. III, Issue 18
These curves will be accepted if you use the single-radius or multiple-radius options. Splines, which are the default curve types for thru points, cannot be used as trajectories for a sweep.
--Thomas G. S. Peterek, Active Design Consulting Inc., Kitchener, Ontario, Canada

A1.2- Vol. III, Issue 18
Assuming you are using Wildfire, use the variable section sweep.
--Niloy Guha, product executive-mechanical design automation, Rolta India Ltd., Calcutta

A1.3- Vol. III, Issue 18
You can overcome this problem by using variable section sweep or swept blend.
--Ravi Kiran, application engineer, CSM Software Ltd., Banglore

A1.4- Vol. III, Issue 18
When curves between two points are created, often the end points of those curves are unable to be perpendicular to the curve trajectory. There are two ways to overcome this problem. After selecting the curve use the trim/extend command and extend the endpoints for a specified distance. This allows for endpoint alignment to a sketch plane because the extension is straight. The drawback to this method is that only a single loop can be used for the sweep.

A second method is creating either a 2projection curve for complex three-dimensional trajectories or a sketched curves. In Sketcher, select the points you would like to go through as you sketch references for placement. You will need a straight section for your start point, so the sketch plane can be created perpendicular to the trajectory. These two-curve creation methods are more powerful in that they will accept multiple-loop sketches and are less likely to fail.
--Lee Hughes, Pro/E designer II, Kohler Co.

A1.5- Vol. III, Issue 18
When you create datum curve thru points and use them for sweep, Pro/E is not able to find adjacent reference surfaces to determine the surface to which your section will be normal. Use advanced option, selecting Feature >Create >Protrusion >Advanced >Swept Blend. After selecting the datum curve as the trajectory, Pro/E will ask you for a surface to which your section will be normal. Show it that surface and you will accomplish your task.
--Yogesh Gaikwad, executive-product design and engineering, Fleetguard Filters Pvt Ltd., Pune

A1.6- Vol. III, Issue 18
The reason you could not select the two-points curve as your sweep trajectory is that you did not sufficiently define the orientation of the curve. Go back and redefine the former two-points curve with its orientations and you will be able to create your sweep with a two-points curve.
--Yang Xue Liang, senior project engineer, Xuzhou Meritor Axle Co. Ltd.

Q2- Vol. III, Issue 18
How can I set the attribute Name as the default instead of Branch in the Locate Common Space Objects window of Pro/INTRALINK? I am using version 3.0 of Pro/INTERLINK.
--Sameeulla Baig, designer, Zamil Aircon, Dammam, Saudi Arabia

A2.1- Vol. III, Issue 18
Usually your administrator is the only one who can set this option but if you have administrative rights, here is what you would do. Select Intralink from the pull-down menu and click on Administration. Select Object >Attributes >Object Attributes. Create an attribute called "Name" if there is not already an attribute with that name. Select the pull-down menu and click on Name and enter the value.
--Jeff Macon, engineering team member, eServ LLC, Rock Island, IL

A2.2- Vol. III, Issue 18
Set up your own locate folder. Here is how to set your computer to locate the latest revision: (clock symbol) & version (clock symbol) along with the name (=). To set up your own locate menu, pick Name (=) and select the plus button on right. This should put it under Attribute >Operator. Select Create and name your setup for Locate. Pick this file, double-click in the value column and proceed as normal.
--Denise Hartranft, designer, Auburn Clutch Division

New Answers to Previous Questions
Q1- Vol. III, Issue 17
How do you organize Pro/ENGINEER files? In other words, which EDM/PDM system do you use?
--Dirk Scherer, PROCAD GmbH & Co. KG , Projektleiter, Germany

A1.1- Vol. III, Issue 17
I use PTC's Pro/INTRALINK.
--Andy Singletary, engineering systems technology manager, Bristol Compressors, Inc., VA

A1.2- Vol. III, Issue 17
We use the Windows NT Server, letting it handle security and permissions. This is accomplished by creating subfolders. One folder is for users to work within, one folder is for the Library data, one folder is for Pro/E and company standards, one folder is for the release process and one folder is for the released "golden" file. Everyone has read privileges to these folders, but depending on their role in the engineering department, users may or may not determine the folders to which they can write. To protect the files, we move them from folder to folder. In Windows NT, we have to copy the files from folder to folder and delete files to allow the file to gain the security permissions of the folder. We have written programs using Excel and Visual Basic to assist in moving files from folder to folder. The system works well, especially if you have no money for PDM. It also mimics the way Pro/INTRALINK works to a certain extent. Users have a workspace, the golden file folder is like common space and the release process folder is similar to the promotion scheme. One problem is the quality of the data. So to ensure data quality, we maintain the history of prior released data in a Zip file. By renaming the Pro/E number on the end of the file, we ensure that data is not lost. Another problem is duplicate data. This system lends itself to using the backup-file command in Pro/E, so most of our user directories are mini libraries. It has taken about a year to work out the bugs and get everyone on board. We are trying to implement Pro/INTRALINK 3.2 at this time with the main goal being electronic signature. So far we have the database running and configured and are beginning to import data.
--Doug Meyhoefer, principle mechanical engineer, L-3 Communications Display Systems, Alpharetta, GA

A1.3- Vol. III, Issue 17
We use MatrixOne as our PDM solution. The MXPRO integration adds a pull-down menu directly in Pro/E and is easy to use for file management and vaulting.
--Emmanuel Stathopoulos, senior mechanical engineer, Hyperchip Inc., Montreal, Canada

Q2- Vol. III, Issue 16
I just received ProE2001 and I am trying to create dimensions. It does not work when I place my new dimensions in Sketcher or on the print itself. Is there a special setting that I need to know about?
--Sue Coupal, drafter II, Eaton Corp., Selma, NC

A2- Vol. III, Issue 16
Select Insert >Dimension > New References and make your choice. There are no sketched dimensions.
--Alejandro Arzate Silva, mold design engineer, Applica Manufacturing, Querétaro, México

2003/05/15

View Manager in Pro/E Wildfire
The new release of Pro/E Wildfire has introduced many new user interface (UI) components and as a result has shifted some commonly used functions. One of the new UI components is the View Manager, which brings together previously separate components into a single dialog box. The components that were in version 2001 of Pro/E included:

(See Figure 1.)

Figure 1

With the new View Manager, some of these components have new names. Simplified Reps is Simp Rep. Model orientation is Orient. Explode states is Explode, and Component display is called Style. The names have changed, but the same functionality remains within the View Manager. The way to get to these components, however, has changed.

To learn the changes, experiment with the available options. One of the most confusing is creating and defining a new simplified rep, explode, orient or style. To do this, choose the New option and give it a new name. While it is still highlighted, select the Edit >Redefine option. This will allow you to define the new view state. When you create a new view state, Pro/E will not have you define that state automatically. You must redefine it.

The View Manager allows you to define view states that include all four view components. You can select from each of the following: Orientation, Simplified Rep, Style and Explode. You also can choose either to explode or not explode the view by using a check box. The check box is available because there is no "unexploded" option in the pull-down menu. (See Figure 2.)

Figure 2

--Submitted by Eric Horn, vice president of research and development, FroTime Inc., San Diego, CA

Creating a T Junction in Pro/CABLING
This technique will show how to create bundles using Pro/CABLING that form a T-shaped junction. Consider the situation shown in Figure 1, where wires form a three-sided branch.

Figure 1

In Release 2001 and later, "branch" bundles can be created to represent T-junctions of wires and cables.

Select Feature >Create >Bundle, and enter a name for the bundle. Select the type of grouping and whether or not it has a sheath. Use Along Path and select the beginning and end locations of the horizontal segment of the "T." Pro/ENGINEER will prompt, "Do you want to include partially routed cables on the path?" Select Yes and use Sel All and Done Sel to select all the wires to include in the bundle. Accept the default parameters or enter new ones. A bundle will be created that encompasses the wires that run along the horizontal portion of the "T." Figure 2 shows the result.

Figure 2

To create the vertical section of the junction, create another bundle and select Branch from the BUNDLE OPTS menu. Pro/ENGINEER will prompt, "Select one or two locations on a top loom bundle to define one end of the branch." Select the two locations on the horizontal bundle where the wires of the vertical portion of the "T" intersect it, and choose Done Sel. Pro/ENGINEER will prompt, "Select a location to define the other end of the branch." Select the location on the vertical wires where the bundle will begin. (See Figure 3.)

Figure 3

Pro/ENGINEER will create the second bundle. When finished, the bundles will intersect in a T-shaped junction. (See Figure 4.)

Figure 4

--Submitted by Florin Neamtu, principal engineer, PTC technical support, Needham, MA

How to Show Bolt Circle Diameter on a Drawing
Frequently designers need to show the diameter of a circular bolt hole pattern on a drawing. Doing this is much simpler than one would expect.

An option exists in the drawing.dtl file that is turned off by default. To show the bolt circle diameter or radius (whichever you used for the pattern), go to the Menu Manager and choose Advanced >Drawing Setup in 2001 or File >Properties >Drawing Options in Wildfire.

From within the Drawing dialog box locate "radial_pattern_axis_circle," and set the value to Yes. Choose View >Show and Erase from the pull-down menus and show axis on the view to which you wish to display the bolt hole circle. (See Figure 1.)

Figure 1

--Submitted by Thomas G. S. Peterek, Active Design Consulting Inc., Kitchener, Ontario, Canada. With thanks to Andrew Burke and Gabriel Martinez.

Showing Various Mechanism Positions Without MDX
In the "Drag Dialog", snapshot the mechanism position, use the "Make Available in Drawing" icon to make the snapshot visible in the drawing. Set and snapshot the mechanism at all the positions you wish to communicate. Make all available to the drawing. A user without Mechanism Design can view the various mechanism states by using the Explode State menu, with the use set at current to pick one of the mechanism snapshots.
--Submitted by Ian Turner, design application support, CSC, MBDA UK Account, Stevenage, UK

Ref. Dimensions in Drawing Mode
Sometimes users receive an error message saying, "Highlighted dimensions cannot be regenerated." (See Figure 1.) When a Reference Dimension misses its reference edge for regeneration of the created dimension, it can become unattached. Delete the Ref. Dim. and create a new one. But you also can Reroute Attached Edge by selecting the Ref. Dim and using the third-mouse button. Hold it and select Reroute Attach and choose the new references.

Figure 1

--Submitted by Palle Srinivasa Reddy, senior engineer—CAD, GE India Business Centre, Begunpet, Hyderabad, India

2003/05/16

Q1- Vol. III, Issue 19
In Pro/E 2000i, what is the best software to create graphical presentations using my Pro/E models? I am finding that models pixilate heavily when I export images as .tif files and open them in PhotoShop. Does 3D Studio or another software prevent this distortion?
--Jamal Shoukry, design engineer, Opus Fena, Buckinghamshire, UK

A1.1- Vol. III, Issue 19
I have found that the best way to export models for presentation is by using capture software such as Capture EZE Pro by Application Techniques, Inc. You can capture the whole screen, just the model window or a part of the window and export to a long list of file types. I prefer .jpg files.
--Frank Johns, design engineer, Newville, PA

A1.2- Vol. III, Issue 19
I've gotten better results using a screen-capture program such as Screenprint than I have by directly exporting images. You can save the images in a variety of file formats including .gif and .jpg.
--Keith Hooks, mechanical engineer, HHP

A1.3- Vol. III, Issue 19
Try rendering the output file as Postscript rather than .jpg or .tif. By doing this, you can control the image size and DPI. I used this method to generate images for a large trade show display and the results were excellent. For those who do not have Photoshop, the output can be viewed using GhostView. GhostView can be downloaded for free. Visit ftp://mirror.cs.wisc.edu/pub/mirrors/ghost/gnu/ghostview/.
--Brett Burdick, manager of product development, Fi-Shock, Inc., Knoxville, TN

A1.4- Vol. III, Issue 19
Making a .tif file requires time for menu selection, size choices, dpi (100-600) and image depth (8-bit index, 24-bit RGB, mono, grayscale). Also .tif files are huge. Instead, I use the Print Screen key function, which creates an image instantly. I paste it into documents (Word, Excel, PowerPoint) and crop it. My screen area is 1,600 x 1,200 pixels and this setting creates fine screen dumps.

To create engineering documents (i.e., GD&T on ECN), I use SnagIt5, which can be found at www.techsmith.com. A windows screen capture utility offers the option of what box zone on the screen to capture; therefore, no cropping is required. You can paste different areas in forms without having to save extra files, or you can save a file in one of the seven file-type options. I open CompuPic from www.photodex.com, paste, "print screen" capture, adjust the image and save as one of the 12 file options for future use in graphic suites—.bmp or .psd or .jpg.
--Carrie Ellen Hall, mechanical designer III, Thetford Corp., Ann Arbor, MI

A1.5- Vol. III, Issue 19
The easiest way to render models from Pro/E is to translate them into .iges or .vrml formats, open them into 3dsmax and then render them. See images below.

Image 1

Image 2

--Chad Waldo, design engineer, R&D Tool and Engineering, Lees Summit, MO

A1.6- Vol. III, Issue 19
Increase the dpi of the output, but remember that doing this makes the file size larger.
--Warren Weber, engineering manager, Bucher Aerospace Corp., Everett, WA

A1.7- Vol. III, Issue 19
I typically use Snagit to get pictures of Pro/E files. The picture will be exactly what you see on the screen and you can save it in a number of formats. You probably can download a test version from www.techsmith.com.
--Claes Albertson, team leader mechanical CAD, Tetra Pak Carton Ambient AB, Lund, Sweden

A1.8- Vol. III, Issue 19
To overcome this problem, simply save (do not export) the Pro/E file as a .jpg. Once you open the .jpg file in Photoshop, you will see it is crystal clear. 3dsmax does the job best, but results vary depending on your graphics card.
--Pratik Madhavji, CAD designer, product developer, London, UK

A1.9- Vol. III, Issue 19
We use MS PowerPoint for presentations. To keep it simple and looking good we use screen capturing. We position the model to the desired orientation and then select Alt/Print Screen. (It's an old Windows trick.) This takes a snapshot of your active window. If you want the full screen, use Ctrl/Print Screen. Just paste the image into PowerPoint or the presentation program of your choice. Once the image is in PowerPoint, you can crop, move and resize it. It looks good and does not become pixilated. If you need a .jpg or tif file format, use Save As and select the image format.
--Chris Novrocki, mechanical engineer, Lockheed Martin, Naval Electronics & Surveillance Systems, Archbald, PA

A1.10- Vol. III, Issue 19
When I export Pro/E models, I export them as .jpgs at 600 dpi. When I open the image in Photoshop, I am able downsize the image without losing detail or causing it to pixilate.
--Matthew Fink, tech manual design, Miller Industries Towing Equipment Inc., Ooltewah, TN

Q2- Vol. III, Issue 19
In Wildfire when I make a sketch, the interface slows or is slow. I have a Pentium4, 560 RAM memory and NVIDIA 32MB card. My graphics are excellent when I spin solid features. What is the optimal requirement for Windows PCs?
--Alejandro Arzate Silva, mold design engineer, Applica Manufacturing, Querétaro, México

A2.1- Vol. III, Issue 19
We had the same problem running PIII 800 with 512MB of RAM and a 32MB video card. We upgraded to the NVIDIA 750XGL (128MB) graphic cards. This seemed to solve our problem. Another thing I did was clear the computer and reinstall everything from scratch. This seemed to help as well. Whenever my computers start acting up and running slow, a good "Format C:" always seems to help.
--Aron J. Oler, senior drafting technician, Belden Wire & Cable - Electronics Division, Richmond, IN

A2.2- Vol. III, Issue 19
Here is the link to the PTC website that shows the minimum and optimal requirements for Wildfire: www.ptc.com/partners/hardware/current/proe.htm.
--Kyle Davidson, Racar International, Anderson, IN

A2.3- Vol. III, Issue 19
Although you have a 32MB graphics card, I have heard from a couple different tech support people that Wildfire is a graphics hog. When you are in Sketcher you are using your graphics memory the most. A smaller card like yours will slow it down. I have an Elsa Synergy II 32 MB graphics card and it does the same thing on all of our machines. I heard the recommendations to run Wildfire are:

I am waiting for two new machines that are a step up based on the above recommendations. They have:

We will see how much it helps.
--Sam Osier - designer, VIASYS Health Care - Critical Care Division, Palm Springs, CA

A2.4- Vol. III, Issue 19
Change your graphics card. I had the same setup at home and the same problem happened to me. Upgrade to at least 64 and it will be OK. But for the best performance get a high-end graphics card such as a Wildcat. The problem does not surface in 3D mode because 3D representatives do not use as much memory as sketches. In sketches, you need more video memory due to accuracy settings.
--Abdul Mukmin Bin Burhan Tajuddin, product development engineer, Siemens VDO Automotive, Malaysia

Q3- Vol. III, Issue 19
Where can I find online tutorials about Pro/E v2001 or Wildfire? I am looking for a complete course in .pdf or .html format. Is it available on CDs and where can I find it?
--Ramanan Selvam, tool design, LuK India Ltd., Hosur, India

A3.1- Vol. III, Issue 19
For online tutorials regarding Pro/E Wildfire, visit these sites:
www.ptc.com/community/proewf/newtools/index.htm
www.ptc.com/community/proewf/newtools/tutorials.htm
www.ptc.com/community/proewf/newtools/personal_productivity.htm
Also, there are often online courses from technical education organizations such as universities. They are a bit harder to find, but are often free.
--Steffen Förster, MCAD application specialist, PTC, ICenter, Central Europe

A3.2- Vol. III, Issue 19
A California company called Frotime has .pdf files and models that you can download. Some are free. Visit www.frotime.com/home.asp.
--James Foster, contract designer, Honeywell Aerospace, South Bend, IN

A3.3- Vol. III, Issue 19
CADTRAIN offers a complete e-Learning curriculum for both 2001 and Wildfire. The CADTRAIN content is web-based, so you can access it from any browser or you can receive it on CD.
--Dave Cohen, vice president, CADTRAIN, Irvine, CA, www.cadtrain.com

A3.4- Vol. III, Issue 19
I've found a brief tutorial for Pro/E Wildfire on the PTC site at www.ptc.com/community/proewf/newtools/tutorials/1/. It is a 21MB Zip file containing an html tutorial showing how to begin using Pro/E Wildfire in the shortest amount of time. The tutorial assumes you are familiar with Pro/E. If you are looking for a complete Pro/E tutorial, visit www1.coe.neu.edu/~zeid/mim3350(spring01)/index2001.html.
--Luca Armellin, mechanical engineer, technical department director, Metelli SpA, Cologne BS, Italy

A3.5- Vol. III, Issue 19
I've had great luck using Google to search "Pro +tutorial". Here's one link I found: www.caddigest.com/subjects/pro_engineer/tutorials_proe.htm
--Kevin P. Alexande, enterprise CAD/PDM consultant, Intergraph Solutions Group, Cincinnati, OH

New Answers to Previous Questions
Q1- Vol. III, Issue 18
Can anyone explain to me why curves created between two points using the "thru points" option are not accepted as trajectory during sweep feature creation? How can I get around this?
--Manohar Dapakara, Eicher Motors Ltd., Indore, India

A1.1- Vol. III, Issue 18
You will have to use the swept blend feature under the advanced protrusion option if the two points are not in the same plane. This is true even though the cross-section of the protrusion is constant.
--Kevin Sullivan, product engineer, Nice Ball Bearings, Kulpsville, PA

A1.2- Vol. III, Issue 18
If you want use the curves that were created between two points using the Thru Points option, you must define the attributes of the curve.
--Grand Fan, mechanical engineer, Casio Electronics Design Center (G.Z.) Co., Ltd., China

Q2- Vol. III, Issue 18
How can I set the attribute Name as the default instead of Branch in the Locate Common Space Objects window of Pro/INTRALINK? I am using version 3.0 of Pro/INTRALINK.
--Sameeulla Baig, designer, Zamil Aircon, Dammam, Saudi Arabia

A2- Vol. III, Issue 18
It appears that you cannot change the default attribute listed for the Locate Commonspace Objects browser. The most you can hope for is to create a saved search and use that every time.
--William Robinson, CAD administrator, Valleylab, Boulder, CO

Q1- Vol. III, Issue 17
How do you organize Pro/ENGINEER files? In other words, which EDM/PDM system do you use?
--Dirk Scherer, PROCAD GmbH & Co. KG , Projektleiter, Germany

A1- Vol. III, Issue 17
We use Product Center by Workgroup Technology, Corp./Softech, Inc. We have been using it since 1997. It works well. It is stable and well seasoned. We are using it primarily for vaulting all CAD data. It does a good job of revision control because it understands the parametric relationship of the Pro/E files. (We attempted to use a directory structure for a while but that became cumbersome, inefficient and hard to control.) We also use Product Center for AutoCAD and CorelDraw files. It is also capable of BOM and workflow tasks. Unfortunately, we have other systems in place for these tasks.
--Bill Pier, supervisor, drafting design, Weil-McLain, Michigan City, IN

Q2- Vol. III, Issue 16
I just received ProE2001 and I am trying to create dimensions. It does not work when I place my new dimensions in Sketcher or on the print itself. Is there a special setting that I need to know about?
--Sue Coupal, drafter II, Eaton Corp., Selma, NC

A2.1- Vol. III, Issue 16
I've run into this situation when setting up new workstations. Check your mouse settings and set the properties on the middle button to Middle Button. This will enable placing dimensions in Sketcher and drawing modes. If the middle button is not set properly, dimensions cannot be created in Sketcher or Drawing modes.
--Rich Miller, designer, Siemens Energy & Automation, Inc., Spring House, PA

A2.3- Vol. III, Issue 16
Your question is somewhat confusing, but if you create a drawing and then choose View > Show > Erase, a window will open that gives you the option to pick different types of dimensioning schemes. This function uses the dimensions that you used in Sketcher when creating your geometry.
--Garry Enyart, designer/CNC programmer, Fort Recovery Industries, Inc., Fort Recovery, OH

2003/05/24

Q1- Vol. III, Issue 20
I was disappointed to find nothing written about Standard Triangulation Language (STL) files in the article "Interoperability Creates Capability" by Tom Kopinski, which ran on Page 12 in the March/April issue of Pro/E: The Magazine. My experience is that this is a neutral file format that never causes problems because it is a simple mathematical representation of a model. The .stl file format handles the geometry as a skin of mating triangles that are only represented by three coordinates (x,y,z). This file format is useful with rapid prototyping machines and high-speed milling machines. I can export this file format from Pro/E, but I'd also like to produce cutter location files based on my .stl model. I can import them into Pro/MANUFACTURING, but the possibilities end there. I cannot place a coordinate system and I cannot select the surface. How does Pro/E handle this problem? Did I do I something wrong or is it impossible to do this? This is important because in the future I think tool and die makers will want to work with the .stl format.
--Jef Verheyen, MCAD user and teacher, De Nayer Institute, School for Engineers

To read the Pro/E: The Magazine article in full or receive other valuable Pro/E information, subscribe to Pro/E: The Magazine at www.proe.com/orderonline.htm.

A1- Vol. III, Issue 20
STL files work great for rapid prototyping when each layer is a few thousand surfaces thick. Smooth curves are not really possible in the process, anyway. The fundamental issue is that it forms curved surfaces with a plethora of triangles. You cannot choose a surface because it is not one surface—it is up to thousands of possible surfaces. A way to reach an approximation is to use more triangles, which can increase file size dramatically. That is one area where an IGES or STEP conversion is superior.
--Al Irion, mechanical engineer, Chipless Metals, Mequon, WI

Q2- Vol. III, Issue 20
How can I edit the default light? It is impossible to sketch a new feature in shaded mode without hanging the light. Using a mapkey seems to be the only workaround, but I would like to solve this problem once and for all by editing the default light.
--Pascal Leroux, industrial design technologist, INO, Sainte-Foy, Quebec, Canada

A2- Vol. III, Issue 20
You have to use a mapkey. There is no other workaround unless Wildfire has something to offer that I do not know about.
--William Robinson, CAD AdminValleylab, Boulder, CO

Q3- Vol. III, Issue 20
Does PTC have a deep-draw, metal-stamping simulation module available for Pro/E Wildfire?
--Ross H. Liberty, owner, Factory Pipe, Ukiah, CA

A3- Vol. III, Issue 20
They have a die module. I design dies. PTC came to our office to do a demonstration. The module was nice for simple progressive and bending dies. If you are looking for software that helps develop the blank size or helps to show where the material could crack, look into second-party software. Check out a company called Automated Analysis Corp.
--Jason Pavloff, design engineer, Cosmos Manufacturing, South Chicago Heights, IL

New Answers to Previous Questions
Q1- Vol. III, Issue 19
In Pro/E 2000i, what is the best software to create graphical presentations using my Pro/E models? I am finding that models pixilate heavily when I export images as .tif files and open them in Photoshop. Does 3D Studio or another software prevent this distortion?
--Jamal Shoukry, design engineer, Opus Fena, Buckinghamshire, UK

A1.1- Vol. III, Issue 19
Re-sampling by 200 percent in Photoshop can help overcome some edge pixilation (jaggies) of a screengrab. TIFF exports from Pro/E offer a higher resolution than do screengrabs. But by selecting Save As and choosing anything other than a snapshot, you will lose customized lighting. We use Okino Nu-Graf software to produce images of models. (See image below.) This process can interpret .slp render files that are exported from Pro/E. It is good value as far as cost. Finished presentations vary in quality. PowerPoint is popular and LView Pro has a handy slideshow.
--David Robinson, Partner, London Associates Product Design, Berkhamsted, UK

A1.2- Vol. III, Issue 19
Please take a look at my PowerPoint presentation by clicking here.
--Mike McGuire, industrial design consultant and principal, Mike McGuire Design, and instructor, Carleton University, Ottawa, Canada

Q2- Vol. III, Issue 19
In Wildfire when I make a sketch, the interface slows or is slow. I have a Pentium4, 560 RAM memory and NVIDIA 32MB card. My graphics are excellent when I spin solid features. What is the optimal requirement for Windows PCs?
--Alejandro Arzate Silva, mold design engineer, Applica Manufacturing, Querétaro, México

A2- Vol. III, Issue 19
I had same problem. Try making a centerline at the beginning of your sketch (anywhere), and you will find that the Sketcher runs faster. In the meantime, we both will eagerly await new machines.
--Antonio Pacheco, superior mechanical engineer/engineering manager, DIMEF, Spain

Q3- Vol. III, Issue 19
Where can I find online tutorials about Pro/E v2001 or Wildfire? I am looking for a complete course in .pdf or .html format. Is it available on CDs and where can I find it?
--Ramanan Selvam, tool design, LuK India Ltd., Hosur, India

A3- Vol. III, Issue 19
Frotime has excellent tutorials that you can download from www.frotime.com. They are well made and very reasonably priced. They cover many subjects from detailing to advanced surfacing.
--Steve Meek, KDM Design & Engineering, Inc., Grand Rapids, MI

2003/06/02

Q1- Vol. III, Issue 21
I would like to set the default shading quality to 10 using config.pro. Is this possible, or do I have to reset it every time I launch Pro/E?
--Marty Ball, manufacturing engineer, Hersey Meters, Cleveland, NC

A1- Vol. III, Issue 21
The answer is in the Level of Detail config.pro options. Add these lines to your config:
lods_enabled YES
lods_value 100
lods_enabled
yes, no
These will determine whether or not the system uses Level of Detail in shaded models during dynamic orientation (panning, zooming and spinning).

When you type "yes", the Level of Detail is enabled. With "no", the Level of Detail is not enabled. You can override this option's setting at run time by selecting Levels of Detail in the Environment dialog box available from the Utilities menu. If Levels of Detail is enabled, the value (lods_value) specifies the default value used to display lods. The value is a percentage of the edge size vs. the total size of the model. Use "smooth_lods" and "yes, no" to work with "lods_enabled" to smooth the levels of detail when a model is shaded. Note that "smooth_lods" and "yes, no" is an optional setting.
--Chris Novrocki, mechanical engineer, Lockheed Martin, Naval Electronics & Surveillance Systems, Archbald, PA

Q2- Vol. III, Issue 21
While using repeat regions for BOM, I want S.No column (& rpt.index) to start with .001 instead of 1. How can I do this?
--Mohan Natarajan, TI consultant, GE India Business Centre, Hyderabad, India

A2- Vol. III, Issue 21
You may be able to accomplish this through repeat region relations. Try changing the text when you switch symbols to something like: asm.mbr.custom_rpt_index. In relations, set rpt.index=asm.mbr.custom_rpt_index and in the next line, multiply asm.mbr.custom_rpt_index by .001. Add custom_rpt_index to your repeat region parameters. I'm not sure if this will work, but it is how we modify entries in repeat regions.
--Brian J. Hart, mechanical engineer, Pro/E administrator, Lockheed Martin NE&SS-Archbald, Archbald, PA

Q3- Vol. III, Issue 21
Using Pro/E 2001,we want to export drawings into AutoCAD because many of our customers still use it. When exporting from Pro/E, it changes the fonts and scales and new dimension creation is not allowed in AutoCAD. How should we handle this?
--Jigar Narendra Talati., director, Hexagon Design Center, India

A3.1- Vol. III, Issue 21
Before exporting to AutoCAD, control the font size and scale through a DTL file in Pro/E. In drawing mode, select advance/draw setup/.

1. Drawing units - mm/inch
2. Drawing text - height

This is how we control font size and scale.
--D. Karthik, Nestech Consulting, Coimbatore, India

A3.2- Vol. III, Issue 21
Export the .drg into .dxf so that the text is intact. Open the .dxf file in AutoCAD and save it as an AutoCAD .dwg file. Check out the config.pro options "dwg_export_format" and "dxf_export_format". You should set this option to 14. By doing this, you will be able to create new dims in AutoCAD.
--Yogesh Gaikwad, executive-product design and engineering, Fleetguard Filters Pvt Ltd., Pune, India

A3.3- Vol. III, Issue 21
I can address the portion of the question pertaining to scale. Pro/E exports all of the drawing entities in paper (draw) scale. It has the ability to create to-scale geometry so long as the geometry is not in a scaled view. Here is an example: Create a 10-inch cube and on the drawing set the drawing scale to 1:1. Create a non-scaled view and a scaled view at half scale. Make sure you have these configuration settings: dxf_out_scale_views yes and dxf_out_drawing_scale yes. Export the drawing and open the .dxf in AutoCAD. Measure the length of one of the edges of the cube in the non-scaled view. It should measure 10 inches. Measure the same edge in the scaled view. It should measure 5 inches. See images below.

Here are some links to related articles from PTC's Knowledgebase:
www.ptc.com/cs/cs_23/faq/det2_faq.htm
www.ptc.com/cs/help/2001/html/usascii/proe/interfac/export_d.htm.

And this is what PTC engineers told me when I submitted a call on the view scale factor: "After exporting either a .dxf or .dwg to AutoCAD, the file is not usable by a AutoCAD user due to a view's scaling factor, applied to "Measurement Scale - Scale Factor". Status details: The current functionality of Pro/ENGINEER will not consider the scale of a view when it is opened in AutoCAD. The scale of the drawing is used."
--Juan Rodriguez, York International Corp., York, PA

New Answers to Previous Questions
Q2- Vol. III, Issue 20
How can I edit the default light? It is impossible to sketch a new feature in shaded mode without hanging the light. Using a mapkey seems to be the only workaround, but I would like to solve this problem once and for all by editing the default light.
--Pascal Leroux, industrial design technologist, INO, Sainte-Foy, Quebec, Canada

A2- Vol. III, Issue 20
I also find it annoying to try and sketch with the default light setup. To change the light select View > Model Setup >Lights. A new window will open that allows you to add/delete different light types. You can change the position, intensity and color of each light. Once you have the lighting set up the way you want, save the settings by selecting File >Save. You can set up and save several light files for different situations. To retrieve a light file, select View >Model Setup >Lights >File >Open and go to where you stored the saved light files. Select the file and select Open.
--Randy Hagen, VIASYS Healthcare, Palm Springs, CA

We are rerunning this answer with a correction supplied by the author.

Q1- Vol. III, Issue 20
I was disappointed to find nothing written about Standard Triangulation Language (STL) files in the article "Interoperability Creates Capability" by Tom Kopinski, which ran on Page 12 in the March/April issue of Pro/E: The Magazine. My experience is that this is a neutral file format that never causes problems because it is a simple mathematical representation of a model. The .stl file format handles the geometry as a skin of mating triangles that are only represented by three coordinates (x,y,z). This file format is useful with rapid prototyping machines and high-speed milling machines. I can export this file format from Pro/E, but I'd also like to produce cutter location files based on my .stl model. I can import them into Pro/MANUFACTURING, but the possibilities end there. I cannot place a coordinate system and I cannot select the surface. How does Pro/E handle this problem? Did I do I something wrong or is it impossible to do this? This is important because in the future I think tool and die makers will want to work with the .stl format.
--Jef Verheyen, MCAD user and teacher, De Nayer Institute, School for Engineers

A1- Vol. III, Issue 20
STL files work great for rapid prototyping when each layer is a few thousandths of an inch thick. Smooth curves are not really possible in the process, anyway. The fundamental issue is that it forms curved surfaces with a plethora of triangles. You cannot choose a surface because it is not one surface—it is up to thousands of possible surfaces. A way to reach an approximation is to use more triangles, which can increase file size dramatically. That is one area where an IGES or STEP conversion is superior.
--Al Irion, mechanical engineer, Chipless Metals, Mequon, WI

2003/06/06

Q1- Vol. III, Issue 22
Our organization has ANSYS and also Pro/MECHANICA. Can anyone offer us general guidelines that indicate when is it best to use ANSYS for FEA and when we should use FEA in Pro/E? Or at least can anyone lead us to documentation that compares the FEA capabilities of the two?
--Rodzaki Mat Saad, Device Analysis Lab, Advanced Micro Devices, Penang, Malaysia

A1.1- Vol. III, Issue 22
It depends on many factors including the goals and complexity of the project, the details of results you would like to achieve and the designer's skills and taste. ANSYS is powerful software for FEA and is capable of solving complicated multi-physics problems. It is especially helpful when combining mechanical, electrical, thermal and fluid features. Pro/MECHANICA is also good, but sometimes limited because it is designed to solve mechanical problems. While the simplest way to perform FEA is within Pro/E, the results are not detailed. Designers should use Pro/E FEA to check their models. If you create simplified models (in 2D or another elementary solid), ANSYS or Pro/MECHANICA modelers are sufficient. For more complicated 3D work, generate the model in Pro/E, import the model into ANSYS and use the FEA procedures. I am not familiar with any references in the extensive FEA literature that compares these three software products. I appreciate and use all of them. Sometimes only personal experience will reveal the unique features of each.
--Zachary Popov, associate professor, department of heat technologies and control, Technical University of Varna, Bulgaria

A1.2- Vol. III, Issue 22
Our organization also has ANSYS and Pro/MECHANICA. The biggest difference between the two has to do with ANSYS' additional abilities to solve the most complex structural problems. If we have a linear-stress problem, we will most likely solve it in Pro/MECHANICA. If the problem has non-linearities, such as stress-dependent properties, we will use ANSYS. Pro/MECHANICA has some capability to solve non-linear problems, such as contact stress (which I really like). But Pro/MECHANICA does not have the range of non-linear capabilities that ANSYS has. If you have ANSYS Multiphysics, you also can solve fluid dynamics problems and magnetic field problems. This can be important, for example, if you are working in an area where you need more than an educated guess at the convective heat-transfer coefficient.
--Dave Maxham, senior member of the technical staff, Tyco Telecommunications, Eatontown, NJ

Q2- Vol. III, Issue 22
Can anyone tell me how to use the style feature or where to find examples that show how to use this feature?
--Vighnesh D. Bhandari, project engineer, QuEST, Bangalore, India

A2.1- Vol. III, Issue 22
A style feature is created by using the interactive surface design extension. A style feature is one feature that contains many pieces of geometry (curves, surfaces and points). It is used to create stylish, curved surfaces.
--Jason Bailey, Sipco Molding Technologies, Meadville, PA

A2.2- Vol. III, Issue 22
Style is a feature provided by Pro/E for creating advanced curves and surfaces. It allows you to create high-quality, freeform curves or directly create curves on surfaces (instead of creating a curve on a plane and then projecting/forming on a surface). Most of this information is available in PTC help.
--Deepak Bhat S., PLM Aerospace, Wipro Technologies, Madhapur, Hyderabad

Q3- Vol. III, Issue 22
How can I run design animation and capture it to a file without showing that it has been made from a simplified representation? I am referring to that message that is on the bottom right-hand side of the Pro/E window.
--Csaba Torok, product design engineer, C3D Ltd., Hungary
No answer yet. Do you know the answer? If so, please send it here.
Please list the question you are answering and include your full name, title, company name and address.

A3- Vol. III, Issue 21
I run into the same problem and I am always going from one to another. As for entering your Pro/E drawing into AutoCAD, I create the Pro/E drawing as a block so I can compare what I have unexploded and dimension it out of scale to the Pro/E block drawing. There must be a better way.
--Michael Contreras, engineering tech III, AMSAFE Commercial Products, Phoenix, AZ

Q1- Vol. III, Issue 17
How do you organize Pro/ENGINEER files? In other words, which EDM/PDM system do you use?
--Dirk Scherer, PROCAD GmbH & Co. KG , Projektleiter, Germany

A1- Vol. III, Issue 17
We use MatrixOne as our PDM solution. The MXPRO integration adds a pull-down menu directly in Pro/E and is easy to use for file management and vaulting.
--Emmanuel Stathopoulos, senior mechanical engineer, Hyperchip Inc., Montreal, Canada

2003/09/11

What's Up With Pro/INTRALINK 3.3?
Pro/INTRALINK 3.3 (released last month) is the first of PTC's data management software tools that is fully compatible with objects created in Pro/E Wildfire. (See Figure 1.)

Figure 1

Pro/INTRALINK 3.3 contains functionality allowing it to take advantage of Wildfire's user interface. One of the most noticeable things is how Pro/INTRALINK interfaces with Pro/E Wildfire. Instead of having a separate workspace or commonspace window open to view Pro/INTRALINK objects or folders, the information can be displayed in the Folder Navigator window inside Pro/E Wildfire. (See Figure 2.)

Figure 2

Workspace and commonspace folder contents are displayed in detail in the Pro/E Wildfire browser window. (See Figure 3.)

Figure 3

The folder navigator allows you to filter the type of files displayed in the browser window and it gives you the ability to hide family table instances, as well. Individual files can be selected and the object will be displayed in the preview section of the browser window via ProductView Express.

To open files, drag them from the browser window directly into the graphics window or simply double-click on them.

It is possible to check in modified objects directly from the Pro/E Wildfire File pull-down menu (See Figure 4.) The Update command also is available in this menu.

Figure 4

Another new functionality with Pro/INTRALINK 3.3 and Pro/E Wildfire is the ability to switch workspaces without having to exit the session. When performing this operation, the only requirement is that you erase all objects from the session.

The way that Family Table objects are handled with Pro/INTRALINK 3.3 has been vastly improved. It is possible to "designate" a file-based attribute of an individual instance. These values can be modified in Pro/INTRALINK instead of having to do the modification inside Pro/E. Also new for family table instances is how the verification state of an object is communicated directly from Pro/E Wildfire to Pro/INTRALINK. Pro/E Wildfire also saves all family table instances to the workspace, even if they have not been verified. When a family table instance is modified inside Pro/INTRALINK, its status is changed to "Not Verified" to let the user know that verification has not taken place on the modified instance.

Pro/INTRALINK 3.3 provides a Resolution Tool to check out versions of family table objects different from those that exist in the active workspace. It is possible to view the versions that are missing from or present in the version in conflict, allowing users to correct the problem in Pro/E and complete the check out.

Other Pro/INTRALINK 3.3 enhancements for family table objects include improvements to the Duplication and Modification functionalities.

Pro/INTRALINK 3.3 has many improvements that allow it to interface with new functionality in Pro/E Wildfire. It may not be long before Pro/INTRALINK and Pro/E become a single software tool instead of two separate packages.
--Submitted by Stan Balish, president and chief executive officer, FroTime Inc., San Diego, CA

Patterns and More Patterns
If you have a feature in which you want to use dependent copies in more than one differing pattern, you normally have to make the dependent copies before you pattern the parent. Otherwise, Pro/E will try to copy the pattern of the parent as well.

There is a technique that allows you to make dependent or semi-dependent copies after you have patterned the parent. The child pattern type can be fully independent of the parent pattern type.

The trick comes when creating the dependent copy of the parent, selecting the feature positioning dimensions and references and selecting the number of occurrences, and setting that to 1, particularly if the parent is a table-based pattern. The child pattern will be created with a single occurrence. You can delete the child pattern (but not the child), which should leave you free to create a new pattern of the dependant child in whichever way suits you.

Another useful technique is to select the same dimension for both the first and second directions, which enables a double-stepped pattern. You also can turn this pattern into a group and then step it (or double step it) in a different direction, ending up with an overall pattern with up to four occurrence values.

Click here to view a PDF that shows two sheets of a quad-repeating pattern. This is a double-stepped pattern in the x direction and double-stepped, group pattern in the y direction. Only the initial bottom left square is a sketch. The second sheet is a modification to show that even the first example can be improved upon.
--Submitted by Patrick Morris, product designer/mechanical engineer, Allied Telesyn Research, Christchurch, New Zealand

Pro/ENGINEER Wildfire, Drawing Mode
There is a hidden dialog box that automates the creation of drawing views. The Drawing View menu manager does not display after this option is applied, and the Insert Drawing View icon is no longer active. All views must be created using Insert >Drawing View after the option is added.

Click: Tools >Options >type new option (it does not appear on the Options list): Option: new_drawing_view_ui Value: Yes > Add/Change > Apply > Close

Insert >Drawing View >General >pick a position for the view >the new Drawing View dialog box opens

You can now select Categories: Type, Visibility, Section, Scale, Representation, View Display, and Origin & Alignment.

View name, Type, and Presentation can also be determined with the new dialog box.
--Submitted by Louis Gary Lamit, instructor, De Anza College, Cupertino, CA. Author-Pro/ENGINEER Wildfire, Brooks Cole Publishing

Speeding Regeneration When Creating Family Tables
When creating family tables, create all the static features and then create the variable features at the end of the model tree. This will speed regeneration because Pro/ENGINEER will regenerate the model from the first variable feature onward. In a model with 20 features, where 10 features are variable, the best result is that 10 features will regenerate where the static features are located before the variable features in the model tree. However if the first feature is variable, then 20 features will regenerate.
--Submitted by Ian Turner, design application support and chairman Pro/UK User Group, CSC, MBDA UK Account, Stevenage, UK

Function Name Changes in Wildfire
I recently installed Pro/ENGINGEER Wildfire and have found the following command name changes:

--Submitted by Karen Thacker, design engineer, Physitron Inc., Huntsville, AL

2003/06/13

Q1- Vol. III, Issue 23
I changed the config.pro with the parameters pro_unit_length and pro_unit_sys to millimeters (mm.n.s). But whenever I create a new part or assembly, the system of units in the Units Manager reverts to inch.lbm.sec. How can I configure Pro/E to create parts and assemblies in mm.n.s without changing the system of units in the Units Manager?
--Alejandro Arzate, mold design engineer, Applica Manufacturing, Queretaro Mexico

A1.1- Vol. III, Issue 23
Pro/E has default templates to start parts, assemblies and drawings. The system uses the inch files by default. If you set a config option template_designasm and template_solidpart to point to the metric parts, all new parts and assemblies will start as metric. There are more templates than just these two. Open the Options dialog box (located under Tools >Options) and type the word template in the Option box at the bottom left-hand side of the box. Click Search and you will see a list of all the templates available. These reside in a directory called "templates" located in the loadpoint directory for Pro/E. The templates can be modified and stored back to this directory or you can create a new set and use the config.pro file to point to the new directory.
--Tom Peterek, Active Design Consulting Inc., Ontario, Canada

A1.2- Vol. III, Issue 23
One way to get around this is to create a Start Part or Assembly. In your Start Part or Assembly, set your units to mm.n.s. You can set up this part any way you like to include special layers, relations, material, parameters, etc. Every time you create a new part or assembly, click (in Version 2001) New >Part. Name your part, uncheck the use-default template and click on Browse. Select your Start Part or Assembly. Your new part or assembly will have all the settings (units, etc.).
--Jeff Macon, engineering team member, eServ LLC, Rock Island, IL

A1.3- Vol. III, Issue 23
You should use a template with the units you want. If you want to use this one as the default template add the template_solidpart option to the config.pro with the path of the file you have created for solid parts. For assemblies, use template_designasm.
--William Quintero, mechanical designer, PROTRAFO Cax, Bogotá, Colombia

A1.4- Vol. III, Issue 23
If you are creating new parts from a start part, check the units. Start parts created before you changed the config.pro parameters will retain the old system of units.
--Bob Fresco, engineering services manager, Honeywell Sensotec, Columbus, OH

A1.5- Vol. III, Issue 23
The system of units depends on which template you are using while creating a new part. If you a have predefined template in which the units are set to mm.n.s, your part will adopt those units. Also take note of the directory where it is storing the config.pro. It should be in same directory in which you are starting Pro/E. In other words, it should load that config.pro to where you have configured the options.
--Yogesh Gaikwad, executive-product design and engineering, Fleetguard Filters Pvt Ltd., Pune, India

A1.6- Vol. III, Issue 23
It depends on which version of Pro/E you are using. In Pro/E 2001, select Utilities >Options. Search for the option template_designasm. Browse and select the file < loadpoint >\templates\mmns_asm_design.asm. Do the same for the rest of the template_options:
template_solidpart < loadpoint >\templates\mmns_part_solid.prt
template_mold_layout < loadpoint >\templates\mmns_mold_lay.asm
template_mfgmold < loadpoint >templates\mmns_mfg_mold.mfg
template_mfgcast < loadpoint >\templates\mmns_mfg_cast.mfg
template_sheetmetalpart < loadpoint >\templates\mmns_part_sheetmetal.prt
Template parts, template assemblies and template mfg models are empty files that may contain datum features such as planes, CSs, points, curves and parameters. Define the units that you want to create or create a new system of units.
--Kaminakis Nikos, applications engineer, INFOCAD S.A., Maroussi, Athens, Greece

Similar answers were provided by George Mantzaflaras, applications engineer, Infocad S.A, Athens, Greece; Sameeulla Baig, designer, Zamil Air Conditioning, Dammam, Saudi Arabia, and Kurt Stark, Alphasem AG, Berg, Switzerland.

New Answers to Previous Questions
Q2- Vol. III, Issue 22
Can anyone tell me how to use the style feature or where to find examples that show how to use this feature?
--Vighnesh D Bhandari, project engineer, QuEST, Bangalore, India

A2- Vol. III, Issue 22
Refer to "Pro/ENGINEER Wildfire for Engineers & Designers" by Sham Tickoo published by Dreamtech Press. This book covers the style environment of Pro/E Wildfire. Tutorials and examples are given that help users apply the style tools while solving standard problems. All the tools available in the style environment are discussed in Chapter 13 with examples. The book will be available June 15 and can be ordered via www.cadcim.com. The book is also available in bookstores in India.
--Abhinav Rai, co-author of "Pro/ENGINEER Wildfire for Engineers & Designers", Dreamtech Press

Q3- Vol. III, Issue 22
How can I run design animation and capture it to a file without showing that it has been made from a simplified representation? I am referring to that message that is on the bottom right-hand side of the Pro/E window.
--Csaba Torok, product design engineer, C3D Ltd., Hungary

A3- Vol. III, Issue 22
The only way I know is to render the animation output. Depending on the length of the animation, this may take a lot of time. You will not see the simplified representation in the animation.
--Dave Simpson, mechanical engineer, Loudspeaker Research & Development, QSC Audio Products, Inc., Costa Mesa, CA

2003/06/23

1- Vol. III, Issue 24
Are there viewers available for download that make it possible to open and view various designs in Pro/E, SolidWorks, Solid Edge, Inventor and Unigraphics?
--Lee Test, production control manager, The Gem City Engineering Co., Dayton, OH

A1.1- Vol. III, Issue 24
I would recommend AutoVUE from Cimmetry. It's not free, but it's inexpensive given the capabilities it offers.
--Ted Smith, account manager, National Technical Support Center, IMAGINiT Technologies, Mississauga, Ontario, Canada

A1.2- Vol. III, Issue 24
Take a look at www.virtuale3d.com/vcollab.asp for information about VCollab. VCollab can be used to import the files from Pro/E, SolidWorks, SolidEdge, Inventor, Unigraphics, ODEAS, CATIA V4, CATIA V5, ANSYS and NASTRAN for high-end visualization. VCollab helps users load large CAD files almost 50 to 75 times faster than most programs and allows users to interact with large data on simple Windows platforms at good frame rates. It also can cut dynamic sections, generate stereo images, measure and mark up data and collaborate visually with remote teams.
--Prasad Mandava, VirtualE3D USA Inc., Richardson, TX

A1.3- Vol. III, Issue 24
Our company has a viewer for STEP files. Most (if not all) CAD systems have STEP export capability. See www.steptools.com/products/stviewer/ for more details.
--Alexey Lipatov, STEP Tools, Inc., Troy, NY

A1.4- Vol. III, Issue 24
Spinfire from Actify will open most file formats. It is not free, but there is a trial with a limit on the number of conversions you can do. Have a look at www.actify.com/v2/solutions/index.htm.
--Sam Worthington, Manchester Science Enterprise Centre, England

Q2- Vol. III, Issue 24
Why does the name on the default home page of the Wildfire browser keep changing (i.e., Hello Dave; Hello Janet, Hello Sanjay)? Sometimes it changes to names of people who do not even work for our company.
--Dave Simpson, mechanical engineer, Loudspeaker Research & Development, QSC Audio Products, Inc., Costa Mesa, CA
No answer yet. Do you know the answer? If so, please send it here.
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Q3- Vol. III, Issue 24
My current project is to identify the development of CAD/CAM in the furniture industry. Do you have any suggestions as to where I might find information regarding this topic?
--Rob Mahurin, student, Mississippi State University, School of Architecture, Graduate Studies Program, Digital Research and Imaging Lab, Mississippi State, MS

A3.1- Vol. III, Issue 24
Steelcase, Haworth and Herman Miller are the largest office furniture manufacturers in Michigan. Steelcase uses Pro/E and has built a great deal of CAD/CAM/CAE technology around the software. I don't have any direct contacts but I'm sure if you visit their websites you could track down someone to talk to. Also, the SMUG (Pro/E Southwest Michigan User Group) has a website and some of its members are from these companies.
--Britt Mott, design engineer, Eaton Corporation, Marshall, MI

A3.2- Vol. III, Issue 24
Check to see if you can contact someone from the engineering department at Flexsteel. At one time they had a company in Dubuque, IA.
--Michael Colson, sales engineer, Northstar Power Co., Ankeny, IA

New Answers to Previous Questions
Q1- Vol. III, Issue 23
I changed the config.pro with the parameters pro_unit_length and pro_unit_sys to millimeters (mmns). But whenever I create a new part or assembly, the system of units in the Units Manager reverts to inch.lbm.sec. How can I configure Pro/E to create parts and assemblies in mm.n.s without changing the system of units in the Units Manager?
--Alejandro Arzate, mold design engineer, Applica Manufacturing, Queretaro Mexico

A1.1- Vol. III, Issue 23
Start parts and start asms contain the units.
--Duane Poe, drafting and design team leader, Leoni Wiring Systems, Inc., Design Center, Columbus, IN

A1.2- Vol. III, Issue 23
Configure your start part(s) and assembly(ies) to the desired configuration. This should give you the results you are looking for.
--Krystal Streib, CAD administrator, MetalTek International, Carondelet Division, Pevely, MO

A1.3- Vol. III, Issue 23
Go to Pro/E dir/templates and rename all inlbs_* files name to mmns_* and reverse.
--Miodrag Bojovic, Mold Designer, Metalka, Serbia and Montenegro

A1.4- Vol. III, Issue 23
To set up units to default to millimeters you have to start earlier from where you are beginning the part. Look at the input box for creating a new part. Does it have a check mark by 'Use default template'? If it does, uncheck it. This will give you a list of the templates that are available for use as start parts. For part creation, there should be four available - an inch and metric solid part template and an inch and metric sheet metal template. The default one is already highlighted for selection. If it is the inch solid part, there are parameters you will have to change in the config.pro to set millimeter part as the default.

In config.pro, there are a series of parameters beginning with template_designasm and ending with template_solidpart. To be consistently metric, each of these values should be set to the metric start part. For example, template_solidpart should contain the value mmns_part_solid.prt. These are the actual names of Pro/E part, assembly, manufacturing or mold files found in the default installation at [loadpoint]/TEMPLATES. All the millimeter file names need to be added or changed for the template_options.

The only complication to this is if the system administrator created a new start part directory with company-created and regulated start parts in it. The config options identify it is start_template_dir. If this option exists in the config.pro (or config.sup) file, you are probably not using the files from the default installation. You will have to look in that directory for the metric template files for parts and assemblies. The names of the metric template files will have to be assigned to template_designasm, etc. The values you now have for pro_unit_length probably are being overwritten by an inch start part. To check, find and open a millimeter part template file. Then go to setup/units. The units should be set to metric correctly.
--David Janes, designer, San Diego, CA

Q2- Vol. III, Issue 23
How do you make a model of a conical compression spring?
--Phillip Fortney, mechanical engineer, LSA Communications, Exton, PA

A2- Vol. III, Issue 23
To model a spring, go to advance feature, then helical sweep. If you want a conical or funny shape, just give it a different profile.
--Min Jin, mechanical designer, Arpeco Engineering Ltd., Mississauga, Ontario, Canada

Q2- Vol. III, Issue 22
Can anyone tell me how to use the style feature or where to find examples that show how to use this feature?
--Vighnesh D Bhandari, project engineer, QuEST, Bangalore, India

A2- Vol. III, Issue 22
Try this web link on PTC's site: www.ptc.com/products/proe/isdx/efs4763/efs4763.htm.
--David Janes, designer, San Diego, CA

2003/06/27

Q1- Vol. III, Issue 24
Are there viewers available for download that make it possible to open and view various designs in Pro/E, SolidWorks, Solid Edge, Inventor and Unigraphics?
--Lee Test, production control manager, The Gem City Engineering Co., Dayton, OH

A1.1- Vol. III, Issue 24
Attached is a JPG of the interface of a viewer program called 3d-tool, which is a fantastic viewer and by far the best I have ever used. What is even better is the price of approximately $200 Australian ($100 US). It runs as a self-contained program (EXE) so the receiver does not need to have a copy of 3d-tool to run the viewer. Just double-click on the EXE file. It supports IGS, STEP, STL, SLP, XGL, 3DS, OBJ, DXF and ASC. I know it works with Pro/E (SLP) and SolidWorks (STL). You can add notes to your parts, colors, transparency, basic animation, etc. The company's website is www.3d-tool.de. To use the tool:

--Michael Cornish, product engineering designer, Cobalt | Niche Design, Victoria, Australia

A1.2- Vol. III, Issue 24
Pro/E has a free desktop to design parts and can open PRT and ASM files. It also has another product that will let you open DRW files. Check PTC's website for free downloads.
--Warren Weber, engineering manager, Bucher Aerospace Corp., Everett, WA

A1.3- Vol. III, Issue 24
Use Delcam's PS-Exchange to view files after downloading and installing. The viewer is free. The actual use of the program is a converter that is expensive to use. It cost $55 for each use.
--John Irvin, president, Neco Inc., Denver, CO

A1.4- Vol. III, Issue 24
There is a company called Cimmetry Systems that has a CAD file viewer called AutoVue. The website says it will handle Pro/E, Solid Works, Solid Edge, Inventor and Unigraphics. The company offers a downloadable 30-day demo.
--Marco Vargas, engineering specialist/CAD administrator, L-3 Communications, San Diego, CA

A1.5- Vol. III, Issue 24
Check out the tool at www.3d-tool.de. The tool reads STL files or render files from Pro/E. You can create a self EXE file that is viewable by anyone without installing the software.
--Jim Gray, Honeywell Control Systems, Scotland

Q3- Vol. III, Issue 24
My current project is to identify the development of CAD/CAM in the furniture industry. Do you have any suggestions as to where I might find information regarding this topic?
--Rob Mahurin, student, Mississippi State University, School of Architecture, Graduate Studies Program, Digital Research and Imaging Lab, Mississippi State, MS

A3- Vol. III, Issue 24
There is a company called Ruskin in Hickory, NC that is using Pro/E and CNC equipment to create wooden chairs rapidly. I have not visited the company, but I heard that it does cutting-edge work in the furniture industry. Our company, Bernhardt Design, is picking up eight seats of Pro/E to convert our process from using 2D data developed in MicroStation. The furniture industry is probably the last industry to embrace CAD/CAM technology. In many ways 3D is not necessary because of the way the industry does business in China. For a company that produces ornate wood products, it is a hard decision to switch to 3D and sometimes the wrong one.
--Zack Lyon, product designer/engineer, Bernhardt Design, Lenoir, NC

Q3- Vol. III, Issue 23
Can you alter a setting to stop DWG creation log files being generated when exporting drawings to AutoCAD format? (An example of a filename is 009304_3_dwg__out.log.2.)
--Scott Ellis, new-product developer, Castalloy Manufacturing, Plympton North, South Australia, Australia

A3- Vol. III, Issue 23
I think there is no setting to stop generating this type of file, but you can try "speakan purge". You can set to delete file types and even customize your directions. The log is useful for debugging errors in DWG.
--Klemen Eržen, mechanical engineer, Ultra d.o.o., Ljubljana, Slovenija

Q2- Vol. III, Issue 22
Can anyone tell me how to use the Style feature or where to find examples that show how to use this feature?
--Vighnesh D Bhandari, project engineer, QuEST, Bangalore, India

A2- Vol. III, Issue 22
Try this web link on PTC's site: www.ptc.com/products/proe/isdx/efs4763/efs4763.htm.
--David Janes, designer, San Diego, CA

Q1- Vol. III, Issue 21
I would like to set the default shading quality to 10 using config.pro. Is this possible, or do I have to reset it every time I launch Pro/E?
--Marty Ball, manufacturing engineer, Hersey Meters, Cleveland, NC

A1- Vol. III, Issue 21
You cannot set the shading level in the config.pro file. You can, however, use a trail file at startup to configure certain options that are unavailable in config.pro, such as shading level. Look on the PTC knowledge base for TPI ID#108201 for detailed instructions on how to use this functionality.
--Dave Simpson, mechanical engineer, loudspeaker research and development, QSC Audio Products, Inc., Costa Mesa, CA