Multiple products with varied part families??

[mpkauto]

Greetings!

I am working on a project that involves multiple (~26) products, each of which contains at least 6 parts that are going to change from each product variation. The only change on these parts will be overall dimensions, and I worked out that I can use the design tables and part catalogs to take care of that. My question is how can I automate the creation of all of these assemblies without building 26 assemblies from scratch?

I've heard there is a way you can generalize constraints by publishing components of a part, and I understand that I'll have to use this as well - I'm just wondering if I can code/use some fancy feature of CATIA.

Thanks!

 

[DBezaire]

If you have the Product Knowledge Template (PKT) module, you can create a document template and add that to the catalog. With the document template you could include detail drawings which would instantiate with the main product assembly.
or
If you do not have this module, you can create a script to preform a File --> New from of this template. This script is easy to follow using tools --> Macro -- Record. You can add this to an icon and drop it on the menus using Customize -- Toolbars - Add commmands - Macros.

Both options create new part UUID numbers and this is the key, other methods will result in instance copies. (other than Save as new, too much work)

Regards,
Derek




Win XP64
R20/21, 3DVIA Composer 2012, ST R20
Dell T7400 16GB Ram
Quadro FX 4800 - 1.5GB

 

[mpkauto]

OK so that's a good tip, I appreciate that - however when I create a new product from the original without recording a macro, it prompts to duplicate the parts in the assembly as well. But it does not do this when I try and record a macro then do this. By the way, I'm using CATIA V5R19 and I have to for the project.

Also, I don't know how to change the code to increment the document name - right now the macro builder will just create a new document with the same name as the one that I record initially. Can someone point me in the direction of where I can find out about Catia and VB interfacing?

Thanks!

 

[ferdo]

Hi,

Copy-Paste in a CATScript, put your "template" CATProduct in C:\temp\ or modify the macro according to your needs. For your question regarding CATIA and VB search in FAQ section for learning programming in CATIA.

Language = "VBSCRIPT"

Sub CATMain()

Set documents1 = CATIA.Documents

Set partDocument1 = documents1.NewFrom("C:\temp\Template.CATProduct")

Dim File

File=CATIA.FileSelectionBox("Filename", "*.CATProduct", CATFileSelectionModeSave)

End Sub

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

 

[DBezaire]

Another method you could use would be parameters at the assembly level.

Create your assembly
In the ASD workbench, pick FX
Create an integer parameter (in my example I also added a string for name control.
Add a formula to the Part Number of the product

String.1 + " " + ToString(Integer.1 )

Since Part Number is a string it would be invalid to add an integer, the ToString( ) command converts integers/reals to strings.

"Bolt " + ToString(Integer.1 )

I hard coded the Nut and Bolt but added the incremental Integer.1 to the formula

Save it in the Temp folder Ferdo had suggested.
Run the macro for New From.

The most important step for naming occurs here. Change the integer number BEFORE you save. This will update the name from what would be Asm_Bracket 1_1 to Asm_Bracket 2

Save Management -->

Regards,
Derek




Win XP64
R20/21, 3DVIA Composer 2012, ST R20
Dell T7400 16GB Ram
Quadro FX 4800 - 1.5GB