How to do it

[Rakesh]

Hi everybody

[Rakesh]

Sorry top question is incomplete and the following is the further information.

I want to do the internal groove with the form tool as shown. This tool have to enter from the centre to required depth than to do the contour to make the internal groove and than come out in X or Y than to clear in Z. How can I acheive this?

Thanks in advance

[Colin Gilchrist]

In Mastercam you can't define a custom tool that had "undercut" geometry like your form tool. You can get code that will work for you you want to cut, but you will be unable to backplot/verify this toolpath, as the tool definition will be bad...

 

The easiest way to do this is with circle mill. Just pick a point at the center of the part. The internal distance between your teeth is 2.147, the OD of the part is 2.0, leaving .0735 clearance per side.

 

So if you were to program a circle mill operation and make the circle you are cutting .147 diameter (you will have to create a "dummy" endmill no matter what), the teeth of your form cutter would be dragging the OD of the part at 2" OD...

 

So take the OD of the part, minus the finish diameter of that groove (let's say 1.5 for example), that gives you a difference of .500 on the diameter. Add that diameter difference to your .147 clearance and that is the diameter if the circle you need to drive. Just make like a .01 diameter endmill, but give it the real feeds and speeds. Make sure you don't use perpendicular entry and set the arc entry sweep to 180°.

 

This will move the cutter over your part (centered), feed down to the depth you set (be careful), Do a 180° arc entry, feed around the circle, do a 180° arc out, then retract.

 

You can even do "multipasses" with keep tool down for your roughing and finishing cuts...

 

HTH,

[Bruce Caulley]

You could just use contour with a start point at the centre. That is what I would try first.

 

Bruce

[Colin Gilchrist]

You could Bruce, but then you would have to worry about messing with lead in/out. Circle mill does it all for you, it is built right in to the toolpath.

 

You also don't need a chain of geometry with circle mill. Just a point and you then enter the diameter into the parameter field...

 

Contour would work but is still my second choice.

[Mike-T]

hmmm... what to do with the comp ?

[shazam/TPP]

Rakesh, do you want to do this on a lathe or mill?? makes a big difference. if mill i agree with Colin.

[Colin Gilchrist]

Mike,

 

Circle Mill has normal cutter comp options. I guess you would probably need to use some type of line/arc combination for comp to work correctly. If so, don't use the 180° arc sweep. I'll play around with it a bit. I bet I can get Vericut to simulate this...

 

I'll give it a try and let you know if I can get it to verify properly in Vericut.

 

Thanks,

[Mike-T]

I don't have a problem with the concept, just figuring that after posting one would have to reverse the comp, and do something with the lead-in-out.

[Rakesh]

Colin and Bruce,thanks for the solution.

Shazam,this job I have to do on mill.

[Colin Gilchrist]

You are welcome Rakesh. Please let us know how it works out.