creating a single part from two assembly parts

[dgiy]

SW 2003 sp3.1

Looking for a good way two crate a single part by combining two parts.

I need to model a part that fits on a gear.

I wanted to insert a part into an assembly and insert a gear from the toolbox.
Then after mating, subtract the gear from the body of the other part so that I am left with a "gear hole".
Is there a way to do this and is there an easier way then the way I described with out modeling the gear myself?

Thanks,
DG

 

[SBaugh]

Sounds like you need to make either a volume or a mold. Either way you need to use the cavity method.

You can use the "Join" command to join to components into one (See help file on this), but you should look at using a "Cavity" to do this. There is no easy way to explain how to do this, but I'll try (without a joined part)

1) Make your part that you want to subtract
2) Make a block that will encompass the entire part
3) Place them both in an assembly.
4) mate the part with a small portion hanging out (You might want to add some extra material just for this)
5) Edit the block at the assembly
6) Click on the Cavity icon or Insert\Features\Cavity
7) Pick the part you want to subtract out of the block
8) Click OK

You should be left with a hull of the previous shape that was inside the block. This works for assemblies to. See the help for clarification.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[jbknudsen]

Agreed, the process is quite simple once you understand what is happening. You are basically telling SW to subtract the gear from the block. This process needs to be completed in the assembly phase as Scott has indicated. Prior to making the cavity, make sure that the part to be subtracted is in the proper position. Under the "help", look for "mold design" as the keyword. Then select "cavities" under that option.

Good luck and let us know how it works for you.

-Jay

 

[JNR]

How about making an assembly and saving it as a part? It might not give you all the histroy you want, but it is simple.

3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......

 

[EdDanzer]

Create the gear, open the sketch that has the tooth geometry, make sure it is fully defined, if not add dimensions until it is, rebuilt the model. Create a new part that needs the gear shape in it. Copy the gear tooth sketch from the gear model and paste it to the face of the new part. Open the gear sketch in the new part and dimensionally locate it where you need it, then extrude cut the shape.