Inserting The Same Component With Different Configurations

[TorsionalStress]

Using Catia V5R19;

If I insert the same part multiple times, can I have some parts with one configuration & other parts with different configurations?

When I change the configuration of one part, the configurations of the matching parts change to the same configuration.

Any response will be greatly appreciated!

 

[KevinDeSmet]

Are you replacing components? Make sure once you have selected your replacement part to change the radio buttons in the little window that comes up asking you to "change every instance of this component".

Certified SolidWorks Professional

 

[TorsionalStress]

KevinDeSmet, I’m referring to configurations inside a single part.

Example, I design a part, configuration (1) without a hole, configuration (2) with a hole. Now I place 2 of these parts in an assembly, I would like one part configuration (1) without a hole and the other part configuration (2) with a hole. Is this possible to achieve?

 

[HGMorgan]

In CATIA, a CATPart can only have one configuration, and every instance of it will be that same configuration. You can't (and shouldn't) have a -1 detail part with different configurations.
I think I see what you are trying to do.
One way would be to create different CATParts with different numbers, for example:
-1.CATPart (finished, complete part)
-1a.CATPart (or -1WH)(same part without hole)
-1b.CATPart (same part different in another way)
-1c.CATPart (etc.)

Create -1 and save. Create -1a and on from -1 and save as different numbers.

Harold G. Morgan
CATIA, QA, CNC & CMM Programmer

 

[TorsionalStress]

Creating multiple files for multiple functions is what I wanted to get away from. I’m very disappointed with how Catia handles, or the lack of handling design scenarios.

 

[DBezaire]

TorsionalStress,
Depending on the complexity there are a couple of ways to handle this. Do you want both parts to show in a bill of material?

Method 1 - Single part
Pro – all construction geometry in 1 part
Con – 3 parts in same file, will not affect drafting, tie view to each body not CATPart. Catia is a 1 part/CATPart type system in best practises.

Inside the CATPart file create a new body called Basepart. When you are finished creating the general part use the copy ? paste Special/as result with link. This will give you a new body. Add your modifications to make Part.B if you want an additional configuration repeat the copy paste special.

Method2 -- Assembly

Create a CatProduct with a CATPart being the basepart. Publish the solid using Tools ? Publications and then copy paste as result with link to a new Catpart added to Product structure. Modify new part to suit your needs. This will give you accurate part weights and allow you to have unique part numbers for a BOM.

Regards,
Derek

 

[TorsionalStress]

My application is as follows;

Welded Bracket which is my (CatProduct) made of;
1. CatPart 1 (qty 1)
2. CatPart 2 (qty 3)

Now I would like to add a hole in one of CatPart 2 after my product has been welded. My detailed drawing will show (part 1, qty 1), (part 2, qty 3) but my final result will show (part 2, qty 2 without a hole) & (part 2, qty 1 with a hole).

Can I use one model, one part number to indicate the different parts without actually designing different parts?

 

[KevinDeSmet]

Well, I would assume Design Tables should get the job done. But I am absolutely not sure so you should do some experimenting.

Certified SolidWorks Professional

 

[HGMorgan]

OK, I mis-understood.
I thought you wanted to show a part in different stages of manufacture. Sorry bout that.
You will need to make a separate part for each configuration.
That is not a shortcoming of CATIA, it's good engineering.
If one part has a hole and the other doesn't, then they are different, and have to have different part numbers.
That is good engineering, and, is required by many procedures (FAA Procedures in my world).
It will help you and anybody that works off of this design to note that "-2 is same as -1 except for assy hole", or something along those lines.

Harold G. Morgan
CATIA, QA, CNC & CMM Programmer

 

[TorsionalStress]

If you think of the application, part 2 (qty 3) does not have any machined features until the end. Why should they be different parts? Catia should offer pre & post part/assembly stages, like SolidWorks!

 

[MarkAF]

Ok, let me recap and see if I understand correctly. You want a CATPart to show different stages of manufacturing? Catia is very capable of doing this, but you'll have to adjust your thinking just a little.

The solution is to create a multi-body part structure. One body for each part contributing to the weldment. Use boolean operations (Assemble, Add, Subtract etc.) to join the part bodies to the top level PartBody. Apply holes, pockets at the level that's relevant. For example, a hole drilled into a single plate would be modeled on the body of just the plate. A hole drilled after the welding ops would be modeled on the PartBody, after the bodies are all joined.

Now, when you want a drawing of the prep material (we do a lot of burnouts at my company), make the drawing view scoped to only that body. The process for that is to create a new drawing view, then click on the body in the part tree before clicking on the face in 3D to create the view.

The method uses one part file for each individual part. Different stages of manufacture are captured and segregated. Drawings of the fabrication process are straightforward to create. In an assembly design context, the final design is represented.

At my company, we have found this to be an exceptionally robust modeling method. I've linked a very simple example part (made in R18). Hope this helps illustrate the principle.


Cheers,
Mark

 

[TorsionalStress]

MarkAF, thanks, this is what I’m trying to do. I’ve never designed a multi-bodied part before but I will take your advice & give it a try.

 

[TorsionalStress]

How does Catia generate a BOM in a part environment, or does this have to be done manually?

 

[marcofa]

MarkAF, can you please show a step by step procedure to create a multibody part and then add features to selected body.
I found only Body command to add body to a part
Marco

 

[MarkAF]

Really there is no BOM in a part environment. HGMorgan's point speaks to this, there is one Part for a Part. If you're after a cutlist, material list, something like that, you should do it manually. (At least, that's best practice in my understanding)

Marco, the basic step is to insert a new body into the part. Then there is a right click option for Boolean operations. To define which level of the part structure you want to work on, pick in the tree and right click, Define in-work object. Now you can add features to the defined level. Beyond that, I suggest you look up the help documents.

-Mark

 

[marcofa]

What difference there is between :
to have many bodies with features like picture Multibodies
to have many bodies after booleans like picture Multibodies2
Marco

 

[marcofa]

Here the second

 

[ferdo]

First one can be transformed very easy in a CATProduct using a CATScript.

Regards
Fernando
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