Hi all
I have built in a document piece, a central piece or is grafted other small pieces, my question is, I would like to recover this small piece with for each of them a document piece to be able to make
the drawing easily and use them later in my way how do you proceed to recover them thank you for your answer.
Marco.
Hello@marco
I'm checking!
You do have an SLDPRT document that contains a set of bodies.
You didn't make all your small parts starting from an ASM in which case you would have an SLDASM file
Kind regards
PS: in principle we use an asm that contains all the individual SLPRT parts files (created separately from the asm) and which will be assembled by constraints in the ASM. This is the simplest AMHA
Yes I preferred to build this way thinking I could afterwards, isolate this small part to make it real independent parts but it's not winning on solidworks I drew on topsolid version lower than version 7 and if my memory is good we built with 2 methods; Said in "place" or "up" I thought not to use the assembly that I don't know very well yet under solidworks but its going to come. That's why we use the method.
thank you again for your answers
Marco
It is possible to build in both methods also with Solidworks but I couldn't tell you more about it
Surely I think too much about workshop assembly ;-) or everything is loose on the editing table but fortunately there is a beautiful shot made by Marco for the editing ;-) ;-)
Kind regards
If it's just taking out the drawings, it is possible to select the body(s) to display in a view (button at the top in the feature manager of the view).
Another method, not much better from a working orthodoxy point of view, is to make configs and delete the surplus bodies.
To make it cleaner, you have to copy the existing part file into as many files as there are parts, edit each file to keep only the right functions, break the external links, build the asm.
Hello @Marco,
To save a part built from several bodies into several independent parts, you have the "save bodies" function available (Insert/Functions/Save bodies). It even allows the part to be converted into an assembly (the parts will then be positioned in space correctly and then frozen).
Hello
The problem with this method is that the bodies are associated with the file from which they came. It is therefore necessary to keep the original file in order to be able to modify.
The basic solution would have been to create an assembly with parts built in this assembly and then save them initially as internal parts of this same assembly (no external file registration at this time).
It is then easier to save them outside while keeping the build tree.
A simple solution is to make different display states: one global one we see everything and one per body.
In the drawing, you just have to choose the display state of a body to see only it and hide everything else.
It's not the fastest but it works quite well.