PRO/ENGINEER 2003年第一季軟體技術文件

2003/01/24

Moving Drawing Views in Wildfire
To move views in Pro/ENGINEER Wildfire, the view must be selected with the left-mouse button and dragged (Selection Filter must be set to Drawing Item and View or Drawing View in order for the view to be selected). To move drawing views using coordinates, select the view and select >Edit > Move Special.

However, by default, the views are locked to disallow accidental view movement.
To unlock views so they can be moved by either dragging or selecting >Edit >Move Special, perform any of these four operations:

1. Set the config.pro option "allow_move_view_with_move" to Yes (default is No) or;
2. Select Disallow the movement of drawing views with mouse icon in the Drawing toolbar or;
3. Select Tools >Environment and uncheck the Lock View Movement option or;
4. With the right-mouse button click on the view and uncheck Lock View Movement.

All four of these operations unlock the views. If the desired behavior is always to be allowed to move the views, set the config.pro option "allow_move_view_with_move" to Yes and this will be used in future sessions of Pro/ENGINEER.
Submitted by Florin Neamtu, senior technical support engineer for PTC Technical Support, Needham, MA

Effectively Using Baselines in Pro/INTRALINK
Starting with Pro/INTRALINK 3.0, baselines only can be created by the user. The system no longer creates an as-stored baseline. It is a configuration available upon object checkout. Baselines are used to retrieve a configuration at a later time. For example, a baseline can be created for an assembly before a new design change is made to retrieve the old configuration at any time.
You can create a baseline in three areas: upon check-in of an object or objects, in Commonspace by selecting Object >Baseline >Create Baseline or when promoting an object. It will then create a baseline of the selected object(s). There are just a few things that you need to input to create a baseline. They are:
Name - Unique name for the baseline.
Description - Description of the baseline created.
Folder - The folder where the baseline will be stored.
Set Optional - This button allows you to select an object(s) in the baseline to be optional. The baseline can exist without an option object but cannot exist without a compulsory object(s).
Clear Optional - This button removes the Optional status and sets the object(s) back to compulsory.
Remove - This button removes the object(s) from the baseline.
Type (optional) - Sets the type of baseline. These options are Read Only, Read and Add, Read, Add and Delete.
Top PIV (optional) - Specifies one object in the baseline whose release level will be used.
Release Level (optional) - Specifies the release level if a top PIV is not chosen.
Protected (optional) - Sets security on the baseline. A protected baseline cannot be deleted.
Public (optional) - Sets the scope of the baseline. Anyone can see a public baseline. If left unchecked, only the creator and administrators can see the baseline.
Once you select the OK button, the baseline will be created. A few tips to keep in mind when creating baselines:
1. Set any object to optional if it is not an important object. These include objects such as hardware, fasteners or any library object.
2. Give useful descriptions so that someone who has not worked on these files can retrieve baselines easily.
3. Avoid unnecessary baselines. Create a baseline of design milestones and important turning points.
4. Do not forget to set the folder. It is best to store baselines in folders that can be found easily. Do not store all baselines in the Root Folder, as this can be overlooked.
Submitted by Eric Horn, FroTime Inc., San Diego, CA

Creating Helical Curves with Elliptical Profiles
While I was playing with curves in Pro/E and wondering if there was a way to create helical curves with elliptical profiles, I looked in a calculus book and saw the analytical equation for the ellipse in 2D:
x = a * cos(theta)
y = b * sin (theta)
a,b are >0
Here is the method:
1. In Pro/E, create the default datum planes and a coordinate system, or create a part with one default template.
2. Select Insert >Datum >Curve >From Equation and pick Coordinate System PRT_CSYS_DEF.
3. Select Cartesian as the Coordinate system type.
4. Write the following in the editor where a=40, b=20, 5*t = how many helical curves you want and 40 is the pitch.
x= 40 * cos ((5 * t) * 360)
y= 20 * sin ((5 * t) * 360)
z= 40 * (5 * t)
When a=b, you will have a circle profile instead of an ellipse. (See Figures 1 and 2.)

Figure 1

Figure 2

Submitted by Kaminakis Nikos, applications engineer, INFOCAD S.A., Athens, Greece

Writing a Text (Extrusion/Cut) over a Cylindrical Surface
Steps:

Submitted by C.R. Subramaniam, Kailasapuram Township, Tiruchi, Tamilnadu State, India

Getting Pro/BATCH Plotting Utility to Work
This program is similar to that of AutoDesk's batch plot utility. As you will see, it is a bit more complicated than drag and drop. The program has not been updated since 1996. Pro/BATCH is intended to work outside of Pro/INTRALINK, so the first few steps must be completed prior to using the software.

Figure 1

1. Create a shortcut on your desktop for Pro/BATCH found in the location shown in Figure 1. If you do not know how to create a shortcut to this file, do the following:
      a. Open My Computer from your desktop.
      b. Browse to the location of pro_batch.bat as shown in Figure 1.
      c. Right-click it and select Create Shortcut.
      d. Drag it out to your desktop.
2. Open the shortcut by right-clicking on it and viewing its properties.
3. Fill in the location of where your config.pro file resides, as shown in Figure 1. You only need to complete this step once. This lets the batch file see your config options for printing. If you fail to do this, printing will be difficult. (You will see lots of datums, CS, thick lines, etc.)
4. Select Apply and OK.

Get the files local to your hard disk
1. Create a new directory on your hard drive. This is the location where you will export your files. I recommend not using your working directory.
2. Check out as usual from Pro/INTRALINK into a workspace. (Drawings, models, assemblies, etc.)
3. Open your Workspace browser window and select Edit. Select All from the pull-down menu.
4. Select Object >Export >To Disk. (See Figure 2.)
5. Select the directory you just created to which you will export. Relationship types should be set to All and select OK.

Figure 2

Start Pro/BATCH
1. Launch Pro/BATCH via the new shortcut you have just created on your desktop.

Figure 3

2. Go to Preferences and set the following as shown in Figure 3. This is the configuration that will work with our laser printer. You only can batch-plot all the drawings in the same size. (Notice the paper-size drop down.) The plotter command line is important: print /d:\\\. The command line for laser printing is the following: print /d:\\lmtds\cadcam4vq. This is different for other plotting devices. (The only space that exists in the command is between the t in print and the /.)

Figure 4

Figure 5

3. Next browse to the location of your exported files. You can do this by selecting the black and blue paper-looking toolbar icon and add the files to the list and Close. (Filter by file type if necessary-Drw, asm, prt.)

Figure 6

4. Fill in the Pro/E command: C:\ptc\proe2001\bin\proe2001.bat or wherever Pro/E exists on your machine.

Figure 7

5. Select File Save. Name the batch file in the space provided and save it. This can be reused if the exported files still exist locally.
6. Under the Schedule pull down, select Start the Task.

Figure 8

7. You can tell Pro/BATCH when to send the prints by specifying 1 hr, 2 hrs, etc. If you type 0, the prints will send immediately.
I have used this procedure only with a laser jet printer. I am unsure how it will work with larger plotters.

　2003/03/04

Scaling in Sketcher
Since the introduction of Intent Manager, many users have struggled while trying to modify dimensions inside Sketcher mode. This occurs when they fail to take advantage of the Lock Scale functionality. With Lock Scale, managing and controlling sketches is simplified and time spent changing one dimension at a time is eliminated. To take advantage of this functionality, you must be inside Sketcher mode. After you create a sketch, it is likely that the assigned Pro/E dimensions are not what you require. (They are usually too large). Changing each dimension, one at a time, can cause your sketch to fail, can make your sketch confusing to look at and can be a tremendous hassle. To avoid the problem, simultaneously highlight all the dimensions in the sketch. Do this by selecting them singly or by dragging a box around all of them. The latter method is quicker and more reliable. Once all the dimensions are highlighted in red, right-click the mouse and select Modify from the pop-up menu. The Modify Dimensions dialog box will appear. (See Figure 1.)
Figure 1

Check the Lock Scale box inside the Modify Dimensions dialog box and make a change to the one dimension listed on the right side that you wish to change. (See Figure 2.)
Figure 2

When you finish the dimension change and have selected the Lock Scale box, select the red check mark inside the Modify Dimensions dialog box and the sketch will regenerate. After regeneration, notice that the dimensions that you did not change in the Modify Dimensions dialog box have maintained their scale in the sketch.
--Submitted by Stan Balish, president and CEO, FroTime Inc, San Diego, CA

Selecting a Range of Features in Wildfire
A range of features or components can be selected to perform actions such as suppress, delete, place on layer, etc. In previous releases, this was accomplished by using the Range option in the menu. In Wildfire, this functionality is available through the Search Tool. Launch the Search Tool by selecting the icon or selecting Edit >Find. Select Options >Build Query and select the History tab. Select the Number Radio Button, and add two rules:

1. Number is greater than or equal to < lower number >.
2. Number is less than or equal to < upper number >.

When Find Now is selected, the desired range is found, and when Apply is selected, the items are selected for operation.
--Submitted by Florin Neamtu, principal engineer for PTC technical support, Needham, MA

A Lost Trick in Assembling Components
Here is how to move or spin a component that is being assembled free of the assembly, and before it is fully constrained. Use the Control + Alt keys in addition to the middle-mouse button (MMB) to spin it and use the right-mouse button (RMB) to move it. This is a good way to get components into their proper position and add constraints. It also works well if you require another constraint and cannot determine the direction of that constraint. Once a constraint is added, the part cannot be moved in a direction that would contradict the constraint.
--Submitted by Kyle Davidson, Racar International, Anderson, IN, (765) 644-4727

Another Way to Create Text on Curved Surfaces
In addition to the method described in last month's Pro/Clues Digital Digest, another way to create text on a curved surface, not only cylindrical surfaces, is to use Offset or Draft Offset. This works well if you also need to incorporate draft on the text.

Create a datum curve with the text. Then select Feature >Create >Tweak >Offset or > Draft Offset. There are other options available to control the feature, but I will not go into detail here. I will suggest, however, that you avoid using Tangent and start with a small draft. Increase it with Modify until you get the desired draft. The advantage to following this method is that you can use it on any surface and it does not require outside calculations
--Submitted by Kyle Davidson, Racar International, Anderson, IN, (765) 644-4727

Showing Various Mechanisms Positions Without MDX
In the Drag Dialog snapshot, the mechanism position uses the "make available in drawing icon" to make the snapshot visible in the drawing. Snapshot the mechanism at all the positions you wish to communicate and make them all available in the drawing. A user without Mechanism design can view the various mechanism states by using the Explode State menu. Use Set Current to pick one of the mechanism snapshots.
--Submitted by Ian Turner, design application support, CSC Computer Sciences Corp., MBDA UK Account, Stevenage, UK

2003/03/05

Using the Trajpar Parameter in Helical Sweep Features
This tip is designed for Release 2001, but will work with 2000i2 as well. The trajectory parameter, also known as trajpar, typically is used in variable section sweep features to vary dimensions. However, the trajpar parameter also can be used in helical sweep features to control the cross section (not profile).
The trajpar parameter varies from 0 to 1 along the trajectory of the helical sweep (0 at the beginning, 1 at the end).
A relation such as sd2=1+trajpar*2. (see Figure 1) would set sd2=1 at the beginning of the sweep and 3 at the end, increasing linearly along the trajectory. The final helical sweep would look like Figure 2.
Submitted by Florin Neamtu, senior technical support engineer for PTC technical support, Needham, MA

Figure 1

Figure 2

Simplify your Pro/E models
This tip is for Pro/E 2001 Build 2350. Overmodeling an object in Pro/E has a number of disadvantages, the most damaging being unnecessary features that are not needed to convey design intent. A common example is hardware such as screws, nuts and fasteners. It may look cool to have your pan head cross-recess screw modeled to exact specifications including every round and cut feature that exists but is it necessary? These features require regeneration time. If enough are present, the extra features may cause a decrease in your machine performance.
If you determine that certain features of your part are not needed but might be displayed graphically, there are a few methods you can use to accomplish this task. One is to replace unnecessary features with datum curves. Datum curves can be created to resemble cuts, rounds, text or protrusions that you typically would create using normal solid features. Using the pan head screw as an example, a fully detailed model of a pan head cross-recess screw could have anywhere from 10 to 15 features on average. The same screw can be made with as few as two features using datum curves to represent the cross-recess feature of the screw. The first feature can be a simple revolved protrusion. (See Figure 1.)

The cross-recess feature can be a projected datum curve. You can sketch the cross-recess section on any plane or surface that is perpendicular to the axis of the screw. Using symmetry and construction lines you can control the cross-recess section using two dimensions. (See Figure 2.)

Select the two top surfaces that represent the top of the pan head screw. This is where your section will be projected. Relations can then be written to control the size of the cross-recess datum curve feature based on the head diameter of the screw. This is useful if a family table is created for the screw. Finally, the color of the datum curve can be set to accommodate your specific needs using >Modify >LineStyle (this is an advantage over using cosmetic text for the feature). The final simplified part with two features should appear as shown below. (See Figure 3.)

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

No Online Help For Pro/MECHANICA?
PROBLEM: Have you ever been in MECHANICA Integrated Mode and tried to get MECHANICA help through the HELP pull-down menu? If so, then you have discovered that none of the MECHANICA manuals are listed in the Contents and Index selection. Although you can access menu-specific MECHANICA help using the right-mouse button on any given MECHANICA menu-pick, you cannot access the top-level index area of MECHANICA's Help page.

EXPLANATION: When installing MECHANICA you tell it where the help directory path is, but this is only used for the Independent Mode. With Pro/ENGINEER Version 2001 and lower you are not able to access the MECHANICA Help index page from within Pro/ENGINEER. Here's a method to make the MECHANICA Help index page available while in the Integrated Mode:

PROCEDURE: Open the browser you use with your Pro/ENGINEER software. Type the path to your Relxxhelp.htm file in the MECHANICA directory. An example is given below for rev. 2001:
      EXAMPLE PATH: D:\Program Files\promech2001\html\usascii\promec\Rel23help.htm
      This is the top-level index page for MECHANICA Help. Once the page is loaded, add it to your Favorite location (bookmark it) in the browser.

IMPLEMENTATION: To use this tip starting with a fresh Pro/ENGINEER session, you do not have to be in the MECHANICA menu. At any time, click the Help pull-down menu and select Contents and Index. Select the new MECHANICA Index link in your Favorites menu after the browser comes up. Alternatively, open your browser apart from Pro/ENGINEER and select the MECHANICA Index link.
I do not know whether this will be necessary within Pro/ENGINEER Wildfire.
Submitted by Randy Speed, president, Speed Consulting, Waxahachie, Texas. Speed is a member of the Pro/E Digital Digest advisory board. To read his bio, click here.

Solving the Problem of Showing Cosmetics on Drawings
You have a drawing with a dozen views. There are some cosmetic features that you have accidentally turned off in these views. You would think it would be a simple task to use the Show/Erase dialog box and turn them back on. No such luck. The detail item button for cosmetic features is grayed out in the show mode. To solve this problem, turn off the preview option in the Show/Erase dialog box. Show cosmetics does not function with preview. To turn preview off, you must select the preview tab from the Show/Erase dialog box, make sure a button other than cosmetic is activated, and un-check the preview box.
Gunnar B Hansen, engineer, damixa, Denmark

Avoiding Linking Problems with Archived Files
Our company has worked with Pro/E for a long time and it has archived many old designs. Occasionally, linking problems arise when we try to retrieve the old designs that link to other files that are archived. This can be particularly frustrating when opening large assemblies that no longer can find files, especially because our early system did not document what some CAD models represented. One way to mitigate this problem is to choose the menu option to open a simplified representation of the large assembly even if you do not know what simplified representations exist in the model. When the list appears, select the option to create a new simplified representation. All of the model names in the assembly are shown without regenerating any geometry. You can determine from the model names in the assembly whether or not it is the assembly you are seeking, and if so you can be sure that all of the models are unarchived before wasting time trying to regenerate the model geometry.
Submitted by Randy Palmer, mechanical design engineer, Government Systems, Isothermal Systems Research, Clarkston, WA

More Ideas on Good Sketching Practice-Comment on Vol. I, Issue 1, Pro Clues 2
I found Kim Cheatham's article, "Learning to sketch with Intent Manager," useful, but I have a couple of reservations concerning the technique. One concern I have is the lack of attention to geometric constraints, which can greatly reduce the number of dimensional constraints required. The method I recommend follows:
As you sketch, points will snap to existing entities and geometric relationships will be applied automatically according to where you move your cursor. This is the Intent Manager making assumptions about your Design Intent. This process is useful and you should search for the constraints. If you do not want the constraint to be applied, move your cursor to a position to where it is not applied and then reposition the point or entity.
Here are some steps to achieve good sketching practices:
Step 1: Use the Sketcher grid and zoom in/out to make the graphics area the same size as your intended sketch. This will avoid problematic bit-by-bit scaling through modification of dimensions in the sketch once it is completed. Large movements of entities will result in extreme distortion of the sketch.
Step 2: Using Lines and Arcs (rather than trimmed circles and squares), start from one point and create the sketch in a continuous line. Trimming circles and squares can result in disconnected end points. This causes open loops that are hard to fix. You also are more likely to create lines on top of lines, which are difficult to detect. Starting from one point and switching from line to arc as you work around the loop ensures good connections.
Step 3: Create the sketch to the correct proportions to avoid resizing work. Drag points and entities to approximately reshape the geometry.
Step 4: Apply geometric constraints. Connect the sketch to the sketching references and use geometric constraints before dimensional constraints to fix its shape and proportions. This will minimize the number of dimensional constraints. The common constraints you will use are tangency and coincidence.
Step 5: Apply dimensional constraints. It is a good practice to try to leave the sketch with no gray, weak dimensions. This ensures all dimensions have been considered and checked.
Step 6: Modify the dimensions. Using the pick icon, double-click a dimension to modify it. Also, using the pick icon you can drag a box around your dimensions to select them and then pick the modify icon to list the dimensions for easy modification. Uncheck the regenerate option because it may cause distortion as each dimension is updated when you make changes.
Step 7: Resolve sketch failures. If the sketch fails it is most commonly due either to disconnection between points causing an open loop-look for weak dimensions of zero or because you have lines on top of lines.
This last issue is the main advantage of creating the sketched loop an entity at a time, continuing from the end point of the previous entity using line and arc segments. This method of creating robust sketches is by no means the only way. There are always exceptions that everyone develops in their own techniques, but I have found this to be a good starting point. Creating robust and successful sketches as the basis of most of the common Pro/E features is a crucial step on the way to a successful model.
Sean Kerslake, department design and technology, Loughborough University, UK

More Help Needed on Helical Springs Clue-Comment on Vol. I, Issue 2, Pro Clues 1
I followed the clue, "Helical Springs Around Non-Linear Trajectories" by Florin Neamtu in the Vol I, Issue 2 edition of Pro/Clues Digitial Digest, and I am unable to create the helical spring around non-linear trajectories. Please advise me.
Harsha Mallikarjuna Thumbaraguddi, design engineer, Praveen CAD Systems, Bellary, Karnataka, India

It's Not That Easy-Comment on Vol. I, Issue 2, Pro Clues 2
Changing the setting of the new_parameter_ui option may not be as easy as the instructions indicated. This option was not even listed under Current Session. Once in Utilities >Options, I had to click the Find button, type in new_parameter_ui, hit Enter and double-click on it when it appeared in the lower window. Only then was I allowed to change the setting from no to yes. In the process of figuring this out, I also found the new_relation_ui option, which apparently performs a similar function for a relations list. It also is hidden and must be changed with the process I outlined.
Jon Smedley, senior product designer, AXXION Group, El Paso, TX

Further Questions-Comment on Vol. I, Issue 1, Pro Clues 1
I have a further question regarding Pro/Clues 1 "File Open Dialog Features." How do I save these settings so they are always there the next time I open a file? If the settings cannot be saved, is it quicker to alt+tab back to my workspace and see what I need to see?
Scott E. Szabo, manufacturing engineer, New Product Development, Ingersoll-Rand Company, Blaw-Knox Division, Mattoon, IL

Answer to Vol. I, Issue 1, Pro Clues 1 Question
No, the settings can not be saved. In my opinion it is faster to use the file open dialog box instead of alt+tab. But it may be faster for you.
Submitted by Stan Balish, president and chief executive officer, FroTime Inc. in San Diego, CA

2003/04/11

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