Pro/ENGINEER Tips & Tricks: Modeling

- Last modified: Jun 23 2003 -

This page is a compilation of tips & tricks related to Pro/ENGINEER. They are not necessarily my own ideas. Use them at your own risk.

Modeling

Modeling a large pattern with surface copies. (20060130)
Reordering Offset Cross-Sections (20010122)
Be carefull with layers
Copying a part with a drawing
Starting new parts or assemblies
Creating a cover by creating a negative shell
Using the Master Model Merge Technique
Exploded Views in R17
Creating your own User-Defined Default Views
How to automate the generation of instance accelerator files for a generic part
John Kudza's (PTC) comments on Ron Davis questions about accuracy.
Rounds

Reordering Offset Cross-Sections (20010122)

Sometimes you find its necessary to reorder the placement of an Offset Cross Section. For instance when you want to reroute the cross-section through other components (assembly) or other features (parts) which were placed after the offset cross-section was created.

The problem with Pro/E is (upto R2001) that these Offset cross-sections are created as Internal Suppressed Cosmetic Features. There is no way to determine its internal ID or to show them in your Model Tree. So you can't select them for reordering to the end of your part for instance.

Here is a workaround to do this:

Determine which feature is immediately before the x-sect. You can do this by redefining the cross-section #modify; 'x-sect'; #redefine; #section) then look at the last feature in the Model Tree.
Now enter the insert mode selecting the previous found feature as the feature to insert after. Verify that the offset x-sect is suppressed by attempting to show it. If it's name is unavailable or if it's not shown then you are at least in front of the X-section.
Create a temporary feature like a coord-sys or datum plane with references only to features early in the feature list, like the default dtm planes or c-cys.
Cancel insert mode.
Reorder all the following features by range (don't select your temp. feature), and reorder them only before the temporary feature you just created.
Delete the temporary feature.
Verify if it was successful by choosing #modify, 'x-sect', #redefine. Then look at the model tree to see that the x-sect is after the last feature.

Tip for PTC: Make Offset Cross Sections a special feature. They should always be the last features in a model. Every new feature must be automatically inserted before it.

Be carefull with layers: The layers in Pro/E are hierachiarchical. Blanking a layer in a top level assembly will blank layers of the same name in ALL components of the assembly. Do a save status after blanking a layer causes ALL components with the same layer in it to be modified and therefor will be saved when the assembly is saved. Leaving you with a lot of models changed unwantedly.
This is especially the case if you use the DEF_LAYER config.pro options to create layers like DATUMS.

Copying a part with a drawing

you can make a copy of a part and a drawing to a new name using the following routine. Lets say you want to make b.drw of b.prt using a.drw of a.prt.

Save a.drw as b.drw
Erase a.drw from memory
Retrieve b.drw
Rename a.prt to b.prt
Save b.drw
Save b.prt as a.prt

Since R17 Pro/E can do this for you. Set the config.pro option: RENAME_DRAWINGS_WITH_OBJECT to BOTH and Pro/E will copy the drawing also if it has the same name as your part or assembly.

Starting new parts or assemblies: It is common practice to start all new parts and assemblies with a set of default datum planes. This makes your part or assembly a lot more flexible. With parts for instance you can only insert before the first protrusion if you start your part with the default datum planes.
In my OCUS archive I added a menu_def.pro and config.pro file which adds two buttons to the main menu. These will start a new part/assembly, create the default datum planes, rename them to appropriate names, create standard view names like FRONT, TOP, etc. and create standard parameters like DESCRIPTION, PARTNUMBER, etc..

Creating a cover by creating a negative shell: When you create a shell you don't have to type in a positive shell value. If you type in a negative shell value material will be added outside your model. This is a neat trick to create a tightly fitting cover of a product.

Master Model Merge Technique Copied from CADTRAIN's INFOCAD bulletin Volume 1 Issue 1.

Do you ever design multi-part assemblies whose shape is defined as a whole using surfaces? Or do you have to create both as-cast and as-machined models of your product? These situations are two typical scenarios where the Master Model Merge Technique can be applied using Pro/ENGINEER.

The Master Model Merge Technique is a method that allows you to include the geometry of one part model (the "Master" part) in another part ( the "Merge" part). The "Master" part geometry is then used to control the geometry of the "Merge" part.

To accomplish this follow the procedure outlined below:

Create the "Master" part model (master.prt)
Create the "Merge" part (merge.prt). Create the 3 default datum planes
Create a "Dummy" assembly (dummy.asm). Do NOT create the 3 default datum planes! (Note: this assembly will be deleted at the end of the process)
Assembly merge.prt inte dummy.asm
Assemble master.prt into dummy.asm. You will have to select the mating references from merge.prt
Select #Adv utils; #Merge from the COMPONENT menu.
Select merge.prt as the part to perform the merge process into.
Select master.prt as the reference part for the merge process.
Select the #Reference and #No Datums options from the OPTIONS menu.
Answer "Yes" to detach master.prt from the assembly dummy.asm.
#Delete merge.prt from dummy.asm and #Erase dummy.asm from memory.
Retrieve merge.prt. It will now have all the geometry that is contained in master.prt.
Save merge.prt. You have succesfully completed the Master Model Merge Technique!

Once the process has been accomplished, you may proceed to add geometry features to the "Merge" part as usual. Any changes made to the Master part will be seen in the Merge part, since they are associated by reference. You will have to reflect these changes by regenerating the Merge part yourself. When the master part is deleted you will not be able to redefine the merged feature, but the latest known geometry of the master part is still contained in the merge part.

Exploded Views in R17

Since Release 17 the way exploded views are handled has been changed and greatly improved. For those of you who don't have Pro/PROCESS for ASSEMBLIES here are some tips on how to handle your exploded views.

These tips were tested on buildcode 9639.

Assembly Mode

General

When you explode an assembly (through #View #Cosmetic #Explode) Pro/E will place all models in an exploded position based on the way they were assembled. The explode position of each component in an assembly is stored within the assembly itself. This also applies to all parts in sub-assemblies further down the tree.

You can now modify your exploded view with #Modify; #Mod Expld. There are two options available to you (the third: Offset Lines is only available in Pro/PROCESS for ASSEMBLIES).

Explode Status

The Explode status allows you to put an individual component back to its unexploded position. Assuming you don't want to explode the components in a sub-assembly you can toggle all those sub-components to an unexploded status by first expanding the entire Model Tree (View -> Expand All) and then select only the sub-models in the sub-assemblies. Do not select the sub-assemblies itself. Temporarily maximize the Model Tree to make the display easier for you.

TIP: Put also your first component in its unexploded state if this was assembled on the default datum planes or coordinate system.

Now we can start putting all the models in a position where you want them.

Position

You will have to tell Pro/E in which direction you want to move your model. You have a variety of possibilities, but the most commonly used will be the Entity/Edge option where you must select an edge or other linear entity or the Plane Normal option. It is important to know that it does not matter what kind of edges or planes you choose. Normally Pro/E can become confused if used edges or planes disappear, but in this case the relative position is stored instead of the way how it was moved. So just choose any edge or plane which gives you the correct direction.

As long as you don't press done in this menu the direction you have choosen will be kept active.

It might be wise to always first use reset to temporarily put a model to its unexploded state and then drag it from there to the position where you want it.

If you want to drag a sub-assembly use the Model Tree or Query Sel to select the assembly itself, otherwise you would select a part of a sub-assembly which you have just put in its un-exploded state and therefor cannot be moved.

If you want to drag several models at the same time set the Move Type in the PREFERENCE menu to Move Many.

If you're familiar with the assembly your modifying don't forget to make use of your Model Tree to select models. This is much faster than query selecting from your screen.

TIP: Store all your assemblies ALWAYS in their UN_EXPLODED state. Before saving always do a #view #cosmetic #unexplode. You could even add this to your 'save' mapkey! If a sub-assembly is retrieved in an exploded state you will not (easily?) be able to get it in an unexploded state in a higher assembly.

Drawing Mode

As soon as you place an exploded view on a drawing the explode positions are taken from the assembly and saved with the view. You will have to modify the exploded state of this view in your drawing from then on. Use #View; #Modify View; #Mod Expld to get to the same menus described above.

But when you want to drag the position of a model in drawing mode the entire display will be dragged (and thus be very slow). This is probably a bug which was still not solved in build 9641. I assume PTC is working on it. Note that although the entire view is dragged as soon as you place the model it gets its new position as you expect and the rest of the models are placed in their normal positions.

So you'd rather modify the exploded view in assembly mode. There are two solutions to achieve this:

Buy Pro/PROCESS_for_ASSEMBLIES. This will keep your drawing views dependant to your assembly explode state until you modify the explode positions in drawing mode. So as long as you leave the exploded drawing view as it is you can modify the exploded view in assembly mode.
Update the explode positions in an exploded drawing view to the explode positions in your assembly by modifying the view type back to un-exploded and then back to exploded. The explode positions in the view will then be restored to the explode positions in your assembly.

TIP 1: Make sure you set the origin of the view to an entity which does not change during the explode process. An excellent element might be the default coordinate system in your main assembly (assuming there is one). This will prevent the view from changing its position relative to other drawings entities (like balloons).

TIP 2: You can create offset lines by showing axes of features of the parts that are exploded an extending these axes with #detail #move and #detail #clip to the desired length. Use #detail #break to make axes skip parts on the same offset line.

For more details check out the paragraph "Creating Exploded Views" in chapter 6 of the "Pro/ENGINEER Assembly Modeling User's Guide".

User-Defined Default Views

You can create your own default 3D views based upon rotating a FRONT view.

Set your model in the desired front view and then rotate it with #view; #orientation; #angles; #horiz or #vert:

TRIMETRIC:
(I don't know the exact equations ... if you do, let me know.)
The proportion of the three sides is approx. 1:3/4:8/9.
ISOMETRIC:
Due to rounding errors in Pro/E you can better use the value: 35.26379
The proportion of the three sides is 1:1:1.
DIMETRIC (my favourite):
The proportion of the three sides is 1:1:0.5.

To create a User Defined Di-metrical Default View add these lines to your config.pro:

ORIENTATION			USER_DEFAULT
Y_ANGLE				-20.705
X_ANGLE				19.471

How to automate the generation of instance accelerator files for a generic part

To generate XPRs for the entire table:

#Part;#Retrieve; the generic
Bring all instances into session for which XPRs are to be generated. Either use
- #Family Tab;#Verify; to bring all instances into session; or
- #Family Tab;#Instance; if only a few XPRs must be created/updated
Select #Dbms;#Inst Dbms;#InstIndex; to update the .idx file
Select #Dbms;#Inst Dbms;#Update Accel; to generate XPR files for each instance in the .idx file.

Rounds: You should select your surfaces for round creation in the respective order in which they were created since Pro/E conducts an order based solution set. If you invert your selections such that the first surface is your second selection and the second surface is your first selection you are causing Pro/E to perform eight times as many calculations to build your round..