Hello
Combines 2 independent pieces to shape one in assembly
Thank you
Hello
If I understood correctly:
1- Insert the parts into an assembly
2- Save the assembly in parts
3- In the room, use the Combine/Add function to merge the pieces
Yves
Hello
If I understand your request correctly, what you need to do to merge 2 pieces into one:
In the file of one of the 2 pieces, integrate the other via "insert" / "part"
It must be set up either by constraint or by displacement (the best is usually the constraints)
With the "combine" tool you can merge the 2 bodies into one if they are at least in contact (this fusion is not essential).
Kind regards
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Hello
Your synthesis is not very clear but we understand the essentials;
What was answered above by the other members is correct, I'll just specify another technique:
You can create an assembly of your first 2 parts on the one hand (-> "assembly1. SLDASM"), then integrate this assembly into a second (-> "assembly2. SLDASM").
By proceeding in this way, when you work in < assembly2>: your two parts are fixed in relation to each other (it moves more) since it is an assembly; So you no longer have the risk of changing a constraint or geometry by mistake.
Want to change the constraints of these parts in relation to each other? Ironed in < assembly1>.
It comes back to the same technique that @gabriel.noesser described to you, the difference is that it keeps a part file (part. SLDPRT) while here it will be an assembly file. Personally I find my way around better this way (because it's more tidy: part file = 1 part anyway/assembly file = mini. 2 parts) but afterwards, everyone has their own way of doing things and that's also the interest!
++
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Hello
@nova141: Is the purpose of combining to make the parts immobile or to have only one reference in the nomenclature?
If this is the first case, use Riky's solution if not rather the first two.
@+
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I answer like Richy
Create your 2 shares Save them independently
Make 1 assembly part1+part2
Save this assembly as part
a lot of problem than the combined tool
if you need to modify it after the fact (thickness side)
- Heavy as the combination tool
@+
Hello, to synthesize or correct some data info.
There are several solutions:
It is possible to create an assembly of the two parts.
If you don't need to make any other changes (I'm thinking of features that add volume, functions that modify geometry like a hull or sheet metal features), then in general this is sufficient.
As for having only one reference in the BOM, there is in the configuration properties the option "display components when used as a subassembly" the hide option allows you to manage the assembly in the BOM as if it were a part.
If you want to merge two bodies because in the end they are only one and the same part, it is possible to make an assembly and then save this assembly as a part, it will be possible to use the combine function. Provided that it is a face-to-face contact, or interference between bodies. Linear or spot contacts are not valid.
Defect, or advantage, of this solution, you no longer have a link with the original parts, so you no longer have the possibility to modify the dimensions, because they are dead bodies (no functions/creation tree).
If you want to keep a link with the original parts (external references) in order to modify the dimensions and have an update of the volumes in the final part while merging the volumes, to add functions such as sheet metal functions (to unfold the volume) or functions adding material, or make a case, then I would recommend using the "Insert/Piece... ".
Advantage, you can retrieve piloted dimensions (be careful, they only recover a dimension, they do not control the geometry), thread representations and information from the drilling assistant, recover or not the surface bodies, retrieve the sketches...
Since we have a link with the original parts, all the modifications made to them will be reflected in the final part (dimensional modifications, geometry modifications, etc.). Be careful, it is possible that after a modification of the original parts, the new functions that have been added will be mistaken.