Showing a part/subcomponent as mirrrored without creating new files?
Showing a part/subcomponent as mirrrored without creating new files?
(OP)
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?
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?





RE: Showing a part/subcomponent as mirrrored without creating new files?
RE: Showing a part/subcomponent as mirrrored without creating new files?
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
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
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. :(
RE: Showing a part/subcomponent as mirrrored without creating new files?
RE: Showing a part/subcomponent as mirrrored without creating new files?
RE: Showing a part/subcomponent as mirrrored without creating new files?
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...
RE: Showing a part/subcomponent as mirrrored without creating new files?
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.
RE: Showing a part/subcomponent as mirrrored without creating new files?
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.
indocti discant et ament meminisse periti
RE: Showing a part/subcomponent as mirrrored without creating new files?
Could u pl tell us how does your PLM system needs it in the BOM ?
RE: Showing a part/subcomponent as mirrrored without creating new files?
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.
RE: Showing a part/subcomponent as mirrrored without creating new files?
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?
RE: Showing a part/subcomponent as mirrrored without creating new files?
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.
RE: Showing a part/subcomponent as mirrrored without creating new files?
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...
RE: Showing a part/subcomponent as mirrrored without creating new files?
It is always pleasure to share knowledge.
All the best lad.
-GEL
Imposible is nothing.
RE: Showing a part/subcomponent as mirrrored without creating new files?
Thanks for the information, and I will let you folks know how it goes.
RE: Showing a part/subcomponent as mirrrored without creating new files?
RE: Showing a part/subcomponent as mirrrored without creating new files?
indocti discant et ament meminisse periti
RE: Showing a part/subcomponent as mirrrored without creating new files?
RE: Showing a part/subcomponent as mirrrored without creating new files?
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.
RE: Showing a part/subcomponent as mirrrored without creating new files?
[URL=http://s21.photobucket.com/user/Tarthrin/media/WOR...]
[URL=http://s21.photobucket.com/user/Tarthrin/media/WOR...]
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.
RE: Showing a part/subcomponent as mirrrored without creating new files?
It is logical that the part features are not display after activation of any Non-Default-Representation . Actually what you have is an instance of a part with the representation of another.
Now, the issue of non show of the Non-Master-Representation, try to associate the attached CATShape file as a representation of an instance and let me know if it displays or not.
-GEL
Imposible is nothing.