External reference 4

[janandk]

Is there a way to create 2 external references from solid bodies without actually doing any boolean operations. When I use the cavity or join command, the solids get automatically united or subtracted. IS there an option to just create external references. Any suggestions will be greatly appreciated. Thanks.

 

[J-C]

Can you elaborate more? Do you want to put two parts into one part file?

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP0.0 on WinXP SP2

 

[TheTick]

Some ideas...

Try grabbing both parts with the same join. I think this keeps the bodies separate.

Instead of join, you might try bringing the parts into a 3rd part fiile using "Insert --> Part".

 

[janandk]

I am trying to design an insert molded part. I do not want to make it an assembly file. I want to bring in 2 solids into a part file from external references without joining them. IS that possible. I could probably use insert-part, but I am having a hard time re-positioning the inserted part. Any suggestions? Thank you.

 

[CorBlimeyLimey]

With practice the move/rotate functions for an inserted part is fairly easy. Keep trying.

or

If you can, upgrade to SW06. It has the ability to position bodies within a part using mates ... same as in an assy.


Helpful SW websites every user should be aware of faq559-520
How to get answers to your SW questions faq559-1091

 

[J-C]

Inserting two parts in to a another part file won't boolean join them, however, if you add material (extrude) then it may merge them. When more than one solid body is in the file, feature will have a box at the bottom of the property manager for which body(s) to apply it to. Usually it auto-selects but you may have to set it to the body you want.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP0.0 on WinXP SP2

 

[engAlright]

If I understand you correctly, what you want to do is create a mould cavity from an existing part without using an assembly (therefore without using the 'Cavity" feature).

To do this:

-create your mould part
-within the mould part, go to Insert - Part - this will let you insert the other part as a solid body in to the mould part
-go to Insert-Features-Combine and choose the "Subtract" option.
-choose the mould part as "Main Body" and the other part as "Bodies to Combine"

When you're done you'll have an external reference from the mould part to the other part (not vice versa).

If you wanted to insert both of these in to a 3rd file, you could just follow the above steps, but instead your first step would be to insert the mould part in to the new file as a solid body (Insert - Part).

Hope this helps.

 

[SBaugh]

There is an option that is not suggested by SW to use, but is avialable to all users.

Tools\OPtions\System options\External References\"Allow Multiple Contexts fopr parts when editing in assembly"

From the help:
Allow multiple contexts for parts when editing in an assembly. You can create external references to a single part from more than one assembly context. However, any individual feature or sketch within the assembly may only have one external reference.

Best Regards,



Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376