Hello
I have several questions about mechanically welded elements:
1- How come I don't have my length in my "welded parts list"?
2- Can we use mechanically welded elements to separate the parts alone, and with the main file to make the name of each part appear with their description in the nomenclature?
For the second question, I tried... But I can't get the parts to appear in the nomenclature. Yet they recognize their parents.
The coin appears in the "Stock-with the unrenowned" tree.
For the length, you have to look at the properties of the bodies in the 3D model.
I'm not sure I understand the second question:
Do you have an ASM that has a mechanically welded part and you want to see the list of bodies that make it up?
You have to choose "Tabulation list" and "Detailed list of welded parts" then expand the side panel of the bill of materials and via right-click on the "mechanically welded" icon choose "Decompose".
From a vocabulary point of view, try to differentiate between the notion of part and body (a part being made up of bodies). From the SW point of view, a mechanical-weld is a part even if by abuse of language we speak of assembly.
Sorry to put it badly...
I was talking about the bodies that make up the piece of welded construction.
Basically what I did on my side: Right click on one of the bodies, and "insert in a new room" (see attachment).
If this is the appropriate method?
Then for the first question, here are my properties attached.
I don't understand why it doesn't show up.
Hello
I think @Stefbeno'm going to explain this to you: but I find this really curious
[[ Right-click on one of the bodies, and "insert in a new room" (see attachment). ]]
As I understand it, there is a hiatus because your body, which is not an independent piece, would have to be inserted into a room or inserted into the same room, which is equivalent to duplicating in the same room and not inserting????
@Stefbeno is right to specify the difference between body and part!
Could you specify what you want to do because the pb may come from there
Kind regards
I have several mechanically welded parts, and in these parts I would have different drilling positioning . To do this, I wanted to separate the bodies and rename them for each mechanically welded element to be clearer during manufacturing. Afterwards, to be able to put the mechanically welded parts in a plan with the nomenclature and the different bodies that I have separated. If this is indeed possible.
Hello
For the 1st question, and I think it started in SW2016 (not sure), it often does it to me. Before, the length column filled in itself, but for some time now, you have to:
1 Click on the "length" column header of the list of welded parts, (see image 1)
2) then go to the left of the screen; in the properties manager and (re)choose "Length" in the "Custom property" field (see image 2)
Normally it fills up automatically
I feel less alone all of a sudden....!! ;-)
A+
Hubert
The "Length" column must be corrected, as @Hubert said.
But above all, you have to create a correct nomenclature model, otherwise the problem will recur with each new drawing.
To do this, record the correct BOM and then point SW to where it is. ("File Location")
"I have several mechanically welded parts, and in these parts I would have different drilling positioning . To do this, I wanted to separate the bodies and rename them for each mechanically welded element to be clearer during manufacturing. Afterwards, to be able to put the mechanically welded parts in a plan with the nomenclature and the different bodies that I have separated. If this is indeed possible. "
All this seems very complicated to me, have you worked with Catia before?
What I would do at first:
With the same body base, if there are only the holes that change (existence, position, number), you can make configurations.
The naming of the bodies can be done at the level of the list of welded parts, which you will use to make the table of the same name in the drawing.
In this drawing, it is simple to display only a body instead of the part (choose "body selection" in the feature manager of the view).
If it doesn't fit, it's possible according to the need (standard mechanically welded base to be adapted to a very large number of customers for example) and if there are only material removals, I'll go for an assembly with assembly functions. It will then still be possible to recover the properties of welded parts.
Thank you all for answering me, and for giving me advice!