Back cutting

[Randy Morton @ Clem Industrial]

Hey all,

 

I am using a custom defined tool (1" EM relieved to .75", .5" from the bottom...so 1" dia. .5 long, then the rest is gone) to do a bore that is 1.25" dia. at the bottom. The hole I have to go thru to get at it is 1.032 (such as is the relieved part of the tool). I told the path to start at Z0 (the bottom of the hole) and contour ramp (.1" per step) to Z.85 (coming back towards the outside).

 

It is not displaying that way (or backplotting). It goes from the top (Z4.2) down to what I assume is Z.85.

 

Any ideas what I have done wrong?

 

[EX-wccprogrammer]

Use a threadmilling cycle.

[crazy^millman]

Or use a standard cicle mill cycle and tell it to start in the center. Most times the cycles do not like to work up. I would use surface flowing for this that was I can control my direction. Then just make sure you pikc the start point as the center of the hole.

 

Problay the best way to know exactly would be old schoool it and draw the toolpath then do a contour with no cutter comp that way you can control everything. If you want the helix then draw it then at you your start and stop draw you in an out to center use 3d for the toolpath opition in contour and be done with it.

 

HTH

[EX-wccprogrammer]

Threadmilling allows use of cutter comp, cutting from bottom up, entry at center of hole, and helical height per rev...

 

This seems to be what you are trying to do....

[dantheman]

You may also try making 1 contour pass at the bottom of hole and than transform that path up?

[Roger Peterson]

Contour Ramp will not allow you to cut from the bottom up. Create the toolpath to cut from top to bottom but in the opposite direction (convention instead of climb). Then right click on the operation in the ops manager - edit selected operations - reverse.

 

 

HTH

[EX-wccprogrammer]

Roger, I did what you described, and it did work. However, it also locked the toolpath so I could not modify it back.

 

Is there any way to remove the lock once it is on?

[crazy^millman]

Yes just click on the op and hit the lock by the ghoost on the operation manager.

 

HTH

[EX-wccprogrammer]

Thanks, the locks have frustrated me for a while now...

 

[Randy Morton @ Clem Industrial]

Roger,

 

Not so sure I follow.

 

You are saying that I should be making a contour toolpath, start at the closest point to the outside, and tell it to feed towards the hole bottom (Z0)? Without ramping this, how can I accomplish this?

 

My tool cutting edge is only .5" wide and the area is 1.35" long...

 

What am I missing?

[TheePres]

Mikey,

That you??

[Roger Peterson]

Select your chain you want to cut, tell it to cut from .85 to 0 in a ramp motion. Then right click on the toolpath in the ops manager to reverse it, it will then cut from Z0 to .85.

 

 

HTH

[Randy Morton @ Clem Industrial]

Got it done. Thanks!

[EX-wccprogrammer]

Yep, it's me... Wuts up Pres?