Slot milling o-ring groove inside a tube

[SlaveCam]

Hello.

 

What's the easiest way to create any circular groove that must be within two Z-values? For a simple example, I have a slot mill of 1.5 width and the width of the groove is 3.5 (from Z-10 to Z-13.5). I could

- create three profile operations with every unique Z depth, or

- create a single profile using depth cuts

 

The problem with both is that I have to calculate top of stock and depth for every tool and it becomes even more onerous with depth cuts. I'd love if Mastercam was able to do the calculations for me

 

Thanks.

[taperlength]

Use Circlemill, check Roughing, uncheck Helical, uncheck Finishing, check Depth Cuts, make Max Rough Step 20.0, # Finish Cuts 2, Finish Step= 1.0, check Keep Tool Down

Then on Linking Parameters Top of Stock= 0 absolute, Feed Plane= 0.5 incremental, Depth= -13.5 absolute.

 

This will take three cuts at Z-11.5, Z-12.5 and Z-13.5

[justchips]

Hello.

 

What's the easiest way to create any circular groove that must be within two Z-values? For a simple example, I have a slot mill of 1.5 width and the width of the groove is 3.5 (from Z-10 to Z-13.5). I could

- create three profile operations with every unique Z depth, or

- create a single profile using depth cuts

 

The problem with both is that I have to calculate top of stock and depth for every tool and it becomes even more onerous with depth cuts. I'd love if Mastercam was able to do the calculations for me

 

Thanks.

You could also transform your geometry to different z depths and chain the multiple levels you want to use. typically driving off the bottom of the tool you have to do some math for the top cut.

 

 

Sometimes, I chain the top chain of the undercut and put a minus on the floor of the cutter width of cut. Ill assign this a different H offset. Than in a different assign the bottom chain of the undercut the normal h number. This is good if you have to hold a tight depth and location for your undercut. 

 

This is a problem that i think deserves it's own path with different variables to define and control the cut.

[mkd]

you can actually Transform along Z.

works great for roughing and finishing passes.

[jlw™]

I just did this today. I'd like to see a dedicated path myself. I always do two contour paths, one with one depth pass at the top with the math for the top to work out then one at bottom depth with depth cuts. Usually I chain the top as zero then do -cutter thickness on parameters page. I'd like to see a path where you chain the top and bottom and put on a desired step down and it figures it out for you.

[Guest]

I just did this today. I'd like to see a dedicated path myself. I always do two contour paths, one with one depth pass at the top with the math for the top to work out then one at bottom depth with depth cuts. Usually I chain the top as zero then do -cutter thickness on parameters page. I'd like to see a path where you chain the top and bottom and put on a desired step down and it figures it out for you.

 

Why would anyone need a programmer then?

 

Seriously, if the software is going to do everything for you.......????

[justchips]

Why would anyone need a programmer then?

 

Seriously, if the software is going to do everything for you.......????

because it's the process you develop not how difficult the software is that really adds value?

[jlw™]

Why would anyone need a programmer then?

 

Seriously, if the software is going to do everything for you.......????

Why have pocketing cycles then?

[jlw™]

The more I think about this the better I like it. Just imagine, top chain, bottom chain, depth increments and done.

[taperlength]

The more I think about this the better I like it. Just imagine, top chain, bottom chain, depth increments and done.

They should add it.  It's already in Lathe and that does roughing and finishing.

[mkd]

The more I think about this the better I like it. Just imagine, top chain, bottom chain, depth increments and done.

I've thought the same thing. there should at least be a Chook for it.

 

but you can basically do it with a rough contour, finish contour and two transforms along z.

 

this method works great if you are doing Hydraulic crescent moon-type cutouts in bores with wheel cutters. Say you have a centerline representing the start point and the endpoint of said semicircle. You can chain in n out (one chain) and one time edit the feed for the in and quadruple for the out. Transform as many as many as needed, all passes with variable feed rates.