Can you Subtract a modelled part from a new part?

[CraigNorms]

I was wondering if it is possible to cut a modelled part out of another solid modelled part.

Example:

A circle saved as a part and then in a new part model say a box. Then subtract the circle from the box. I know this is a simple example and their is an easy way of modelling this, but say it was a more complication modelled shape.

If anyone can help, that would be great.

 

[Heckler]

You can combine multiple solid bodies to create a singled-bodied part or another multibody part. There are three ways to combine multiple solid bodies:

Add. Combines solids of all selected bodies to create a single body.

Subtract. Removes overlapping material from a selected main body.

Common. Removes all material except that which overlaps.


Best Regards,

Heckler
Sr. Mechanical Engineer
SWx 2007 SP 2.0 & Pro/E 2001
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(In reference to David Beckham) "He can't kick with his left foot, he can't tackle, he can't head the ball and he doesn't score many goals. Apart from that, he'

 

[CraigNorms]

O right ok, the only trouble is the combine tool is greyed out can I only use it in a particular way!!!

Thanks!!!

 

[Theophilus]

Sounds like you're in an assembly. If so, simply save your assembly as a part (.sldprt) file and then do it.



Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe transcends reason.

 

[CorBlimeyLimey]

If you are in an assembly, you can use the geometry of the new part to create a sketch (or surface) which can then be used to cut 'material' away from the old part. This would be classed as "in-context" or "top-down" modelling.

If you need to do this strictly in a part, you can use the Insert > Part command to add the new part into the old part, and then do the boolean subtraction using the Combine tool.

 

[CraigNorms]

Thanks for that!!! its working ok now. I was in a part modelling but it didn't grey out. Working now though, probably Solidworks doing something funny. Thanks again.

 

[J-C]

It will be greyed out if you only have one "Solid Body" in the part file.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2006 SP5.1 on WinXP SP2
SolidWorks 2007 SP2.1 on WinXP SP2