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Bodies relations to each other

Hi, I'm new to the concept of bodies. I'm trying to create what would be a welded assembly in a part document by unchecking the command "Merge Result". This create different bodies. I would have prefer not creating bodies but I need them to get different haching in the layout (is it the best way to do it?). I don't want to do real assembly to get less files. Now, I try to relate the sketchs of diffent bodies to each other with relations but it doesn't work. Is it normal? The bodies need to be fully independent without geometrical relations to precedent sketches? Also, if I uncheck the Merge Result and then change my mind and check it back, it is still impossible to put relation between the active sketch and the precendent sketches. Solidworks seems to bug. Can you help me? Thanks JC

Reply to
Primeau
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It would seem to me that you are trying to force SW into a corner that is not where it wants to be. My suggestion would be to go ahead and create the assy and let the system work for you, rather than fighting it. I think you will be much happier in the end.

WT

Reply to
Wayne Tiffany

It seems you want assembly functionality with a Part Feature Tree. This can be accomplished but you have to resort to more files.

Don't worry you won't have to remodel anything to accomplish what you want

1) Insert > Features > Split In the split tool there will be a list of all of the bodies in the Part. Double click each body and it will give you the opprotunity to save it to a separate part file. while doing this you can save 2 parts out to the same file but be careful of parts that are mirrors of eachother because it seems that SW body checking wasn't up to snuff and it confuses mirrored bodies for instanced bodies I haven't rechecked in current releases but I had a minor issue with this 6-8 months ago.

2) Now that you have saved each body out to it's own part file. RMB on the split feature and it gives you the option to create an assembly. Click that option. Now you have an assembly of the bodies in your Multi-body part file. If you edit the new assembly you will notice that all the parts are fixed in place. If you make them floating you can apply mates and move everything with mates.

Corey

Reply to
CS

(P.S. You will be able to edit the individual parts by editing the origional multibody part. and the individual parts will update.) If you only want to make minor movements you can also use Move/Copy body in the multibody part without an assembly.

Corey

Reply to
CS

Why not create a weldment part (file->new->part, then open the weldment toolbar)? SW will automatically handle the bodies as separate weldment members, generate cut lists, explode the part and allow ballooning, allow different xhatching, you also get automated gussets, automated welds, etc.

Regards,

Reply to
Anonymous

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