in need to create a new part within an existing assembly of multiple parts. I'd like this new part to be the volume of empty space enclosed by two of the existing parts in this assembly. how can I create this new part?
It would be quite easy to create this part by saving your assembly as a part file ( File > Save as > select .sldprt as the file type), then use the intersect tool to gain the enclosed volume as a separate body. You could then mate this into your existing assembly if required.
To do it all in the assembly, you would have to create a new part (Insert > Component > New Part) then you can use the Offset surfaces, set the distance to 0 and copy the surfaces of existing parts in the assembly. Finally knit them together and form a solid.
thanks for response logan.
I followed what you said up to the pt where you said to use the knit tool. After the new part was created by picking the surfaces of the existing parts, I then used the Insert, Features, Intersect (within the new part) to create a solid part from the surfaces. Thanks very much for your help!!!
Disclaimer: I have not tried this.
My approach would be to save your current assembly as a completly different name. That why you can go back to what is golden after trying this out if it does not work.
Create a sub-assembly of all those parts in your current assembly, then open the sub-assembly as it's own stand alone assembly.
Save that assembly as a .step file.
Save and close everything out.
Import your new step file into a Solidworks session and only chose the surfaces. There is your part of the volume you want.
PRO/E is a lot easier. You just save it as a lightweight assembly.
thanks for your response john frahm.
Please see the att. assembly
I created an assembly with 3 parts in it. The part #3 will be changed to whatever you make changes to part #1 and part #2
I used features on part #1 and Part #2 to build part #3 - so basically I adapted part #3 to part #1 and Part #2
thanks for your response, Christian...this sounds like what I'd like to do. I will try today!
Christian Chu - example would be my pick as well, however I would control everything with a sketch part embedded in the main assembly and all the parts would be tied together using that Sketch Part.
Agreed - There are several ways doing this and master sketch sure is a way to build a robust assembly with more parts. I created a quick assembly to demonstrate the ability of using the ref. parts to build a new part.
There are many different ways and I think it's awesome when we get so many different answers - the OP can take a pick - depending on the project...
If there are only 3 parts, then multi-body is also a good choice for "quick and easy" approach
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