Creating multiple models with user-defined dimensions

[FlyDeltaJets]

I'm not even sure what this would be called, hence the somewhat confusing subject title, so I'll try to explain the best I can.

Let's say I want to build an assembly that has many different sized I-beams. Is there a way to setup a generic I-beam shape within Pro/E and then whenever I add a new beam into the assembly, a dialog box prompts me for the specific dimensions (i.e. flange, thickness, web thickness, height, length)?

Thanks in advance!

 

[robertib]

You may want to search the help files for Flexible components.

This will allow you to create a generic part, and use different parameters. The only problem with this way of doing it is that using Wildfire 3.0 & later, all of the different components show up as the same part in the BOM (if you use the part name - it works OK is you only use a description).

Otherwise, create a family table of the I-beams (excluding length) & make the length flexible - this will have the same effect as above, but will have the different I-beam sections collected together.

 

[fighterpilot]

DeltaJets,

Yes, setup your standard I Beam model and then use Pro/Program to generate a new one each time. With Pro/Program you can specify the dimesions, parameters, etc you want the user to specify and Pro will build the model accordingly. This works well but make sure your model is robust by flexing it to make sure it will regenerate at the extremes and use relations to control the items that need to stay in proportion.

Family tables and Pro/Program each have their pros and cons. You'll need to investigate both to determine which will work best for you.

--
Fighter Pilot
Manufacturing Engineer

 

[FlyDeltaJets]

robert,

I've got the family table created, but how do I go about making the length flexible? Is this something that's done in the "generic" part model?

 

[robertib]

What you need to do is to go to the Edit -> Setup -> Flexibility, and select the dimensions you would like to alter.
If you are going down this route, then I would recommend to rename the dimensions to something readable (instead of d8, etc).
The way to do this is to right-click on the feature in the model tree, and select Edit.
Highlight each individual dimension, right-click & select Properties.
Go to the second tab, and change the dimension name (eg d8) to something more relevant (eg width).