[lew90nicis]

Hi guys,


I need some help from the CamWorks/Solidworks experts out there...

I've created an assembly in Solidworks, that consists of the fixture and two parts that sit parallel to each other. I want to use only one operation to machine both parts but because they are two separate parts in the Solidworks feature tree, CamWorks creates a separate operation for each part.

Is there a way of doing this?

Many Thanks in advanced.

John.

[extanker59]

I don't use Assembly very often so there might be a better/easier way but, when I wanted to face all my parts together one time, I made a sketch in the assembly on the face of the first part and made the line end after the last part. Then in the feature tree added an open profile, etc...
Hope that helps
Chris

[Japazo]

Are the parts identical? If so, why are they two different items in the feature tree? Can you just replace the second one with the same item as the first and program as usual?

If they are not identical, there isn't much you can do. Either do what extanker suggested or attempt to pattern a toolpath from the first part to the second. If the parts are not identical, it is good practice to take the time to program them individually rather than putting band-aids in your programs. It can save some serious headaches down the road, for other people if not for you.

[lew90nicis]

Hi guys, thanks for the replies. The parts are different. They are two open ended pockets, where the open sides face each other with a 30 thou gap between them.

I wanted to run a pocketing operation that continued from one part to the other, working from outside to inside. Instead of pocketing one part then moving onto the next part.

Is there no way of converting the two parts into one part whilst leaving the gap between them?

[extanker59]

Do the same thing as the line but use a pocket instead. You just have to program it in assembly.

[lew90nicis]

Sorry Chris, I don't quite understand what you mean.. Can you explain how you do this please.
Many thanks.

[Japazo]

Draw a sketch in the assembly for the pocket you want to machine. Insert it as a pocket feature into one of the parts. While still in the operation tree, right click on that operation and select "assembly feature". That will prevent CWx from making multiple instances of the feature. You should be able to generate the toolpath as you normally would and adjust the toolpath as necessary.

[extanker59]

OK, here's how I just did a test. Create a sketch of a pocket you want on your top surface of the tallest part (or any plane parallel). Anything closed. Then go to the CAMWorks feature feature tree tab. There you will find the part manager with your Mill Part Setup. Right click on the Mill Part Setup and insert a Pocket and "Use: Assembly Sketches", pick the sketch you just made. After that it's all the same except that you have to go down to the Set Up after the stock manager to generate operation.

[lew90nicis]

Cheers guys! That's perfect! Thanks ever so much!