ASSEMBLY FEATURES IN V5

[kadego]

Hi Group
I have a welded assembly modeled as a CATProduct.
There are more than one instance of some CATParts in the assembly. eg ITEM-01.1, ITEM-01.2
One complete face of the assembly has to be machined flat.
I tried using INSERT >ASSEMBLY FEATURES >SPLIT with a plane located in a separate fix constrained skeleton CATPart.
I only want to split ITEM-01.1 However ITEM-01.2 is also affected.
Is this normal? How can I just split ITEM-01.1?
I want to avoid having different CATParts as this will cause me problems when it comes to creating a BOM.
Anyone had this problem? Anyone got a solution or should I be doing it some other way?
TIA
Dave

 

[solid7]

Yes, this is completely normal. The assembly split affects all instances. It's really just a method to introduce a part operation at the assembly level.

The ideal way to do this, if it WERE POSSIBLE (it is not) would be to have he ability to copy and paste an assembly (as result with link) into a part file, where the operations could be managed.

Sorry. We've all been there.

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[jackk]

I think you have to make a new CATPart for the machined version of ITEM-01 part.

 

[solid7]

It's easy when you have parts designed in part context. You can use the "copy as result with link" option. But you definitely have to make some part configurations for assemblies.


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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[kadego]

Funny thing is I was led to believe that Catia was a high end CAD software.
Does anyone know if there is anything in the pipeline to fix this shortcoming?
Dave

 

[solid7]

Funny thing is I was led to believe that Catia was a high end CAD software.

And what makes you think that it's not? Have you used any other portion of the software? You can't get just get angry and level an accusation, because it doesn't do somehting that you want it to, the WAY you want it to.

For any example that you can give me of a weakness, I can probably show you 2 things that it does better than another "high end" software.

It's not such a small product that you can declare it bad, just because it doesn't do one particular task the way you expect it to.

Does anyone know if there is anything in the pipeline to fix this shortcoming?

I'm not so sure that this is viewed as a "shortcoming". It would be great if it worked differently, but I suspect that it is a logical working created intentionally, for the sake of some other process.

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[DBezaire]

Kadego - An instantiated copy of a part is an exact duplicate, change one part and you change them all. It's your methodology that is the problem. By your above description - they are 2 similar parts with only the stock ordered different.
Option 1 - Make a second CATPart, copy paste/ result with link to part "B" Make a parameter part "A" add a formula to put the parameter in the description property box. Add a formula in part "B" to add the parameter from Part "A" in the description box of "B". Now part "B" is a linked copy (incase of change), add your machined face.
Option 2 - in the product copy/paste special - break link. This makes an exact duplicate with no links to original. The disadvantange, if part "A" changes you will manually change part "B".

Regards,
Derek

 

[kadego]

I am not angry ....just amused that it doesnt support something so basic.
I use NX and V4 and there is no doubt that V5 is the best in so many ways above the other two.
No need to get so defensive, it was tongue in cheek.
Do you not agree that it is a feature that should be there?
All the best to you
Dave

 

[solid7]

Do you not agree that it is a feature that should be there?

I wasn't angry! (internet forums don't convey emotion well)

I can't say that I agree or disagree. Like I said earlier, it may not be a shortcoming. Since I'm not a programmer, I cannot say.

It may very well be that I'd lose some other valuable functionality at the expense of this feature - in which case, it would need to be a value judgement that I'm totally unequipped to make.

Does that sound better?

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CAD design engineering services - Catia V4, Catia V5, and CAD Translation. Catia V5 resources - CATBlog.

 

[Akesson]

The problem that you have is an issue that you share with many other users and companies.
If you for an example work a lot with weld assemblies that should be machined after welding maybe Catia V5 is'nt the best CAD software. ProENIGINEER handles this very good but many other issues worse than V5.

As far as I know there are workarounds to this problem but not any solution.

The reason is (I've been told from Dassault) is that a CATProduct can't contain geometry (some programming mistake done early in the developing phase of V5???). E.g not able to contain planes and points.