Showing a part/subcomponent as mirrrored without creating new files? 2

[Tarthrin]

This question is related to the symmetry function of CATIA v5.

We have some thermistor wires that are the same part in the real world. In the CAD they are routed symmetrically from each other. I want to show the second part in the right place/orientation, but without creating a new part document (it messes with our PLM system BOM)

We also can't use the variant feature in CATIA if it creates new geometry.

Anyone got any ideas?

 

[sudhakarn]

Can u tell me what issue you are facing while you are making the symmetry in CATIA ?

 

[Tarthrin]

Let me try to explain the issue in an example.

I have an assembly. ASM-001
Inside this assembly is two instances of a wire that gets plugged in. WIRE-001

This is what I want
ASM-001

-WIRE-001​

-WIRE-001​

(shown in mirrored position)

In the assembly there are two instances of WIRE-001. However, the way the wire is routed is mirrored. So in order to show this I take the first instance of WIRE-001 and use the assembly symmetry feature.

Now a new part "Symmetry of WIRE-001" is created.

So the BOM looks like this now:
ASM-001

-WIRE-001​

-Symmetry of WIRE-001​

Now my bill of materials is messed up.
When I try to save this assembly into our PLM system it has to treat the symmetry part as a seperate 3rd part.

 

[jopal]

Can you not turn off the symmetry instance to not show up in bom by checking off the "visualization in bill of materials" option

 

[Tarthrin]

I think turning off the "visualization in bill of materials" works in the drafting mode in catia. The problem is that the PLM system does not recognize that option. It looks at the structure of the the files to determine what parts and what quantity are included in an assembly.

 

[ferdo]

Hi

Why you not create the symmetry inside the part itself? In this way you will have a single part with all what you need inside...

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

https://picasaweb.google.com/103462806772634246699/

 

[Tarthrin]

The only problem with that is then the BOM only shows one parts instead of 2 copies of the same part.

I have thought about doing the symmetry inside the part, and then just overlaying the symmetrical part. That way it would look correct, but it would be a little chintzy.

 

[itsmyjob]

on the chintzy side, I wonder if you could just have 2 of your part in your assembly, then with a script modify the matrix of one of them to an indirect matrix.
if Smarteam check position matrix it could be weird.
BOM is OK, it is looking good also in 3D but I won't be surprised with side effects.

Eric N.
indocti discant et ament meminisse periti ​

 

[sudhakarn]

Hi,

Could u pl tell us how does your PLM system needs it in the BOM ?

 

[GELFS]

Hi Tarthrin,

what you need is a part with two different shapes (ie representations iaw CATIA terminology).
The solution to the problem is as follows:
1. Insert in both positions instances of the same Part-Product (ie WIRE-001)
2. At the second instance associate a different representation.

If you need more help just let me know.

-GEL
Imposible is nothing.

 

[jackk]

Please explain more GELFS. These is a new topic for me.

What are "representations"? How do you create these shapes and how do you choose which shape is shown?

Besides symmetrical parts, what are representations used for?

 

[GELFS]

Hello JackK,

Before going to the topic "Representations", I would like to clarify the following in order to avoid any misunderstandings.

Representations are not connected to symmetrical parts. The real design intention of Tarthin is have one part with two different topologies and symmetrically positioned (look at the uploaded image of first post where the two parts he is speaking about are not identical) instead of having two parts mirror-symmetrical to each other. That is why, I proposed to him to not use mirror-symmetry but instead to insert twice the same part and to assign a different representation to one of them.

Having clarify this, let’s been involved on your questions
“What Are Representations Used For?”
The answer is simply the following: Whenever we need the instances of a specific part to look differently between each other (i.e. to have various representations) within one product or in different products.

Some examples are the following:
1. A Flexible Hose (or any part with some flexibility) is a part with a specific part number which most probably must be inserted in a product many times and each of these instances must look differently. Then we need the single part to have several representations.
2. Some
3. A part like a Heat Exchanger can have several representation like:
a. “Solid-Full and Detailed Representation” used for the production of the manufacturing drawings.
b. “Simplified Representation” used in the mechanical arrangements and for routing of distributed systems like pipes and cables and for the production of composite drawings. In this case we need our components to have “light” representation otherwise we overload out products with unnecessary details.
c. “Insulated Representation” when we want to make space analysis.
4. A Cabinet or a valve can have the following representations
a. “Open Representation” in case the valve or the door of the cabinet is open and when we want to make functional or space analysis.
b. “Closed Representation” in case the valve or the door of the cabinet is closed
5. In Process & Instrumentation Diagrams (P&IDs) we have the need to insert a valve where in some places is Normally Closed (NC) but the same valve in some other place is Normally Open (NO)
6. Some parts, like metallic Cable-Trays in shipbuilding, of a specific type have just one part number for each type all over the project although their length is slightly different from place to place. Then one solution to this problem is to have one part with different representations and in BoM to appear the position nr, the part number and the length of it.

To create a shape
[File] > [New] and in the |New| dialog box select [Shape].
To attach a new representation to an instance of a part in a product:
Open a Product and change to the |Product Structure| workbench. Select an instance in the product and click the [Manage Representations] icon. In the |Manage Representations| dialog box click [Associate] button …
To define the active Representation use the [Activated] column in the previous dialog box.

I hope it helps.


-GEL
Imposible is nothing.

 

[ferdo]

Hi

Hats off for explanation, star from me. Still, he need to check if his PLM system can handle this, for what I met along the time, the right choice was Eric proposal...

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

https://picasaweb.google.com/103462806772634246699/

 

[GELFS]

Salut Ferdo,

It is always pleasure to share knowledge.

All the best lad.

-GEL
Imposible is nothing.

 

[Tarthrin]

This sounds very promising. Now that things have settled over here for a few days, I will have to give this a try.

Thanks for the information, and I will let you folks know how it goes.

 

[jopal]

When I go to File-New I do not have the option for [Shape].

 

[itsmyjob]

CATShape is only available with a license for one of the following products: CNA.prd, EQT.prd, HGR.prd, HVA.prd,
PIP.prd, RCD.prd, TUB.prd, WAV.prd (they are the shipbuilding products and you can find their full name under
Equipment&Systems.

Eric N.
indocti discant et ament meminisse periti ​

 

[Tarthrin]

I finally had time to sit down and try this out today, and lo and behold, we don't have the right licensing to use "shapes" ...

 

[GELFS]

Hello Tathrin,
may be is not necessary to have CATIA Applications licensies.
Try the following:
- Open your CATPart (WIRE-001) with the first representation and change it so as to look like the second representation
- Save it with different name (WIRE-001_Rep2.CATPart)
- Change the extension of the file WIRE-001_Rep2.CATPart to WIRE-001_Rep2.CATShape.
- Now try in a CATProduct which includes an instance of WIRE-001 to attach to it the second representation of it.

Pls let me know if you succeeded with this rework.




-GEL
Imposible is nothing.

 

[Tarthrin]

Getting closer. Still not quite there yet.




I have a piece of foam that is shown in its applied position and its flat pattern position.
I saved a copy of the contoured part and made it flat, and named it ST-001350-FLAT.CATshape
In the assembly I used manage representations to associate the catshape file.
It seems to take, but when I try to activate the catshape, nothing shows. Also note in the tree where the part features would be shown, nothing is shown under the part when the catshape is activated.