Hello
My problem is the following:
I have a volume piece which is itself divided into several volumes. (see image)
I would like to integrate it into a mechanically welded assembly without it dividing this part into several folders in the list of welded parts.
So the 3 blue folders in one so that in the drawing there are not 3 lines for one and the same part.
Is it possible to do this while keeping this list in automatic?
Thank you for your answers.
Hello
You integrate this part directly into the welded construction or you make an assembly and then you integrate your welded construction and then your solid part ???
The cubic part (image 1) is integrated into an assembly (image 2), it is in this assembly that I want to have only one folder in the list of welded parts, for one part and not 3 like the 2nd image.
For me it seems logical but it's not easy to explain, I hope you understood me.
The "mechanically welded" environment is a part in SW and not an assembly.
I assume that you insert your bevel by the function command/insert part. You may be able to modify your angle gear so that it has only one body (even if it means making a configuration)
That's what it seemed to me, hence my question. Normally, if you make an assembly and you put the mechanically welded part and then your volume part, you will only have your two parts in the shaft with the stress file...
You are right.
I have a custom library of solidworks on a server, I just drag the parts I want to integrate but it comes back to the same as the insert part function.
I thought about this solution but the problem is that it also loses the materials related to each part of the cube that I want to integrate. I would like to keep this to have a real weight and characteristics in the end. I don't know if that's possible.
What do you think?
The assembly keeps the materials if they are entered in the parts, if you make a nomenclature you will see the weight and the material of each part...
I reiterate what I said just before, it's not an assembly, I insert my part into another room, so there are 2 pieces in one.
For weight, you can assign a material to a specific volume body in a room.
If your imported part has very different bodies (like the plastic body and the steel chucks, so the COG is very offset), and you modify your imported part to have only one body, then this effect of offsetting the COG cannot be recreated.
If you apply a material at the level of the fused body-group, as stefbeno points out on the cdg, it also distorts the mass, and starts to create defects (especially if the details, the interior void of the part are filled, simplified).
As commercial parts are often multi-material, or with interior empty spaces (which are sometimes filled-simplified-filled in 3D), their density is extremely variable: 5.6 / 6.2 / 6.7 / 9.0... And this also affects the position of the CDG.
It will be more appropriate to start with an "ASM in hybrid mode", to include the PRT-Const.Soudée, and to add the components of the trade (Bosch, etc...), with ASM nomenclature in tabulation (BOM-ASM-TAB)
If the choice is made to stay on a PRT-Const.Soudées, when you make modifications in the 3D (change the order of the parts, marker, etc... while remaining in Automatic mode) you sometimes have to delete and then put the table back, because it doesn't update all the time with certain 3D modifications (unlike the ASM).
Warning: if someone is just starting to work with the soldered PRT-Const., it is not recommended to disable the "Automatic" mode, as this may lead to errors in the Soldered Const.table that will not be the fault of the software!
The simplest would therefore be to make an assembly directly rather than a mechanically welded assembly.
Thank you for your answers,
Have a nice day.
It depends on how this part is attached to the rest:
- if it is "welded", you have to agree to "tinker" to compensate;
- if it is bolted, it must be switched to normal assembly.
even welding, it is possible by using a:
- "ASM in hybrid mode" (with a PRT-Const.Welded in it)
- and use a BOM-ASM-Tab.
In addition, ASM mode is a thousand times more reliable than PRT mode, for repositioning components.
(the movement of a body with constraints, in a PRT has been bugged since almost the beginning of the function... and never seems to have evolved...)
Olivier42, how did you create an ASM in hybrid mode? just put the part in construction welded in it or is there a manipulation to do?
Yes
first in your PRT-Const.Welded you have to leave the "list of welded parts in automatic!! "
then we create an ASM,
one slips in "one or more PRT-Const.Soudée",
we slip in the Components of the trade (Bosch, etc...)
in a MEP, we put a view of your ASM,
then we select the view, and right-click add ASM nomenclature (= BOM).
Then we click next to it, to leave the BOM panel,
Then we re-select the BOM, to have the complete menu (and yes that's how it is)
and we choose the classic and usual options of an ASM nomenclature, i.e.:
Grouping: On / Mode 3
check: follow / follow...
And because we want the "Hybrid ASM" mode, in "BOM type" we exceptionally choose Tab, then we choose the numbering mode.
then afterwards by wanting to put bubbles, on different views,
before placing a bubble, do "properties" on the view, and check "Linked to the nomenclature" and choose the right one...
Thank you Olivier42 for these explanations, everything works perfectly except for a line in the nomenclature table that had been created without anything in it. I deleted it and everything is perfect.
Problem solved.
Have a nice day.