How to speed this operation up

[MIL-TFP-41]

I keep thinking I am missing something simple here...but here it goes. Been doing quite of bit of medical parts as of late...and they all have this similar feature. Its a counter-bored hole, .215 dia X .09 deep, then going down to a .198 dia .04 deep. What has been working great is roughing with a 3/16 drill and then using a ramp contour or helix bore with a 1/8 endmill.

 

This is where I am trying to get a few extra seconds....after ramping out the .215 dia, mastercam wants to rapid back up the the clearance plane, then feed back down to the start height of the .198 dia. Realize that I do have my plunge rates set at 200IPM and the machine can rapid at 2000IPM, but when traveling such short distances (Clearance plane is only .100 above the part) it does not accelerate to this speed. What I would like to be able to do is ramp/helix the .215 dia the go ahead and ramp/helix the .198 dia without going back up to my clearance height until the .198 hole is done. Cutter comp must be used (total tolerance of the holes is .001). I know this will only save maybe 1-2 seconds per hole....but when you are talking 1000's of holes it adds up.

 

I have tried making my own helix's for mastercam to follow....but along with being a PITA to create, they come in as a spline which makes the program much longer than it needs to be.

 

 

Any ideas????

[Stan_z]

try to do the operations together and use the incremental depth and keep tool down if using depth cuts

[Guest]

Create them as 2 separate operation and use the tool path editor to remove the the rapid retracts

[MIL-TFP-41]

quote:

---

Create them as 2 separate operation and use the tool path editor to remove the the rapid retracts

---

We got a winner....thanks a bunch!!

[jeff]

What about having a special drill/mill ground to the form that you need?

one tool does it all.

If it cuts to size, you would save a lot more time that way especially if you have thousands of holes.

Otherwise, hand edit the rapid moves is the best way as pinky suggested.

[Code_Breaker]

Try this with a single toolpath under 'linking parameters' (note numbers are suggestion):

 

Checked Clearance and absolute at 2.0 Checked "Use clearance only at the start and end of operation"

Checked "Retract" and incremental at .100

Checked "Feed Plane" and incremental at .050

 

HTH

[robh]

why not use a 3/16 em instead of the 1/8?

[Cad-Camr]

Im with Rob. Bigger End Mill, maybe 5/32. Also the ramp contour IMO is very inefficient for time. I also use incremental to machine multiple depths in the same cut. I've never tried John's suggestion but It sounds worth a try.

[mkd]

sorry interpolation boys, jeff is right; port tool always win for production speed.

especially on cnc with weak servos (like haas) that are slow to accelerate

[Kyle Waters]

on some of the older controls, switching from rapid to feed for short moves actually costs you time. You may get a bit more by keeping the G1 and using your max cutting feedrate.

[K2csq7]

+1 to Form Tools