PDA

View Full Version : designate rapid path?



declanhalpin
05-09-2013, 04:06 PM
Ok, one more question:

I am cutting a piece held in an "Alligator-Jaw" clamp - it's very long & skinny, and allows the material to be milled around the profile. The problem is my machine doesn't have enough Z-travel to get up & over the clamp, I have to go around it. Is there any way to force MC to follow a particular path when rapiding between roughing/finishing?

I do know about creating an STL of the clamp, but that won't work. I am using a keyseat cutter to cut inside the top-down footprint of the clamp. And since MC doesn't support keyseat cutters I'm telling it I have flat endmill of the same diameter. This large, imaginary endmill causes a collision with the clamp STL, whereas the real keyseat cutter does not.

dh

turmite
05-09-2013, 11:21 PM
Dh the quickest way I can tell you is to use cut along curves and build the tool path like you want. That way you will not get crashing, collision etc. You could also use the cut along curves to make the cuts with your keyseat cutter, just be sure you have your offsets correct.

Mike

ps you might want to post a zip of your file as well as a drawing of your cutter.......

JOM
05-10-2013, 01:31 AM
You can also edit the toolpath directly by moving the control points on the toolpath curve.

1) Select the toolpath.
2) Set control points on in Rhino.
3) Edit the control points on the rapid traverse curve.
4) Set control points off.

184322
184324

/Joakim

declanhalpin
05-10-2013, 07:19 AM
Thanks, guys. I tried both of those solutions, but neither is great:

Turmite's solution: The feed speed is quite slow, so using cut along curve takes a LONG time to get the cutter to go where it needs to go. What should be a 1:30 operation becomes a 5:00 routine.
Joakim's solution: Each toolpath (roughing, finishing) only has 1 Z-level, so there is a plunge and a retract, but no rapid shown in the toolpath.

Dan B
05-10-2013, 08:43 AM
Could you edit the G-code to speed up the move between cuts? I know that's not the best solution, but it should get the results you want. Is it possible to post the model so we can take a look?

Dan

svenakela
05-10-2013, 08:47 AM
Make it as two separate paths?

declanhalpin
05-10-2013, 11:56 AM
Thanks, as always for everyone's help!

Yes, I suppose I could edit the G-Code but this will be an on-going issue with this clamp, and I'm going to have to teach others how to handle it. I'm hoping for an alternative fix. Svenkala, the routine is already in two paths. The problem is it's a 1-pass operation, so no Rapids are created.

I've attached a file showing what I mean, hopefully it will help.

tx!!

svenakela
05-10-2013, 01:16 PM
Thanks, as always for everyone's help!

Yes, I suppose I could edit the G-Code but this will be an on-going issue with this clamp, and I'm going to have to teach others how to handle it. I'm hoping for an alternative fix. Svenkala, the routine is already in two paths. The problem is it's a 1-pass operation, so no Rapids are created.

I've attached a file showing what I mean, hopefully it will help.

tx!!

Ah, that's quite easy to fix. Make a polyline for each rapid (like your arrows) on the Z height you want to travel at. Reselect the tool but set the speed to 9999 or whatever speed is fast enough for ya (don't forget to save the tool to set the speed). Create a path with the Along Curve-command, Ramp depth 0 and Ramp angle 90. Sort the paths in the order you want, in your case Toolpath 1, new "Rapid" 1, Toolpath 2, new "Rapid" 2 back to the start position.

You get my idea? I can make a vid clip later if you want.

Dan B
05-10-2013, 01:32 PM
Maybe in cases like this it's worth having a permanent "rapid tool" in your tool library. Then you don't have to worry about changing your default speeds and feeds (and having to change them back after). Just pick the "rapid tool" and follow the rest of Sven's suggestions. Keep it the same tool number so you don't do any superfluous tool changes.

Dan