Tool Changes

I was hoping someone could shed some light on this or maybe even a bunch of people and I can get a few ideas.

How do you go about tool changes? e.g. I have a part that is 13 mm thick and am going to cut it out of a board that is 20 mm thick. It also has small pockets and
mounting holes in it. I would like to use a face mill to knock it down to a thickness of 13 mm. Then change tools to a 1/8 Flat end mill to create my mounting holes and pockets. I am using fusion 360 and can see how I would change the endmill for each toolpath. I just don’t understand how to manually do it without affecting my end product. This scenario is of course fictitious and is just an example. No file to share.
-What steps would you do to make this happen?
-How would you change the tool and resume where you left off?
-Can we use a Z Probe with our MPCNC’s? (If so, how?)

Here is the process I use:

  1. Z-probe : I use the z_min limit wiring from the RAMPS. One wire goes to a plate, the other I clip to the router bit. If you home the Z, it will touch the plate, raise a bit, then lower again and stop. This is the surface of my stock+touch plate. In my case my touch plate measures 10.3mm.
  2. G92 Z-10.3 : This sets the surface of my stock to 0mm.
  3. Set X,Y : Move the router up a bit then to the origin I want to set as the start of my job. Note in fusion 360 when you setup your job, make sure you configure the “setup” of the job in CAM to the same origin.
  4. G92 X0 Y0 : The x,y and will now be set to 0. You can return to this location by typing G1 X0 Y0, then G1 Z0 (I do them separately otherwise it will follow a direct path to the original and I don’t want the Z to lower until I am over the origin).
  5. Run your fist tool path.
  6. G1 Xsomenumber Ysomenumber Zsomenumber : Use this to move the router to a spot that you can reach easily to do the tool change.
  7. Shut off the router.
  8. Change the bit.
  9. G1 X0 Y0 : move to over the origin.
  10. Hook up your touch plate again and repeat steps 1,2.
  11. G1 Z10 : move the bit up
  12. Remove touch plate.
  13. Run your next tool path.

Hope this gives you an idea. If you don’t already have one, google gcode descriptions and find a listing of what all the gcodes do. That’ll help a lot. Also, if you are using Repetier on a PC you can save some of these as scripts if you use them frequently. Unfortunately, the MAC version of Repetier does not have the script buttons :(.

Good luck.

>>Edit - I found that it used the last feed rate for all my G1 moves, so I usually specify the speed I want the moves to be. For example : G1 X0 Y0 F2000.

I’m still working on an M6 solution that I’m happy with so in the interim, I do pretty much what P3DCNC described.
Right now, I find exporting each tool as a separate gcode file the easiest way to keep everything straight as I work.
So my folder might look like project_001_3mm_Endmill.gcode, project_002_1mm_Ballnose.gcode, project_003_3mm_Vbit.gcode, etc.
Makes it easy to keep machining operations in correct order, and I can ensure I’m changing to the proper bit.
The important thing is to make sure your steppers stay locked throughout or you’ll probably lose position.

Thanks guys. This is exactly what I was looking for. I’m ordering a touch plate

Have a look at the estlcam videos. He shows fancy stuff and even foil tape as a touch plate. Might as well start cheap and easy and see if you want something bigger.

Foil tape… That’s genius. I will definitely check out the videos. Thanks Ryan.

Yeah, the foil tape is an awesome idea. I figured that I’d try it and see what happens.
I had assumed that the bit would pierce the foil when you zero, so 1 use and done.
Nope. It’s so sensitive it literally touches the foil and stops, no mark. Even with a vbit. I find the adhesive fails because it gets sawdust on it between uses before the foil gets screwed up.
Unless you forget to remove your clips and home the machine, then the foil will tear. ahem

I didnt realize that a touch plate was so primitive. I don’t know why, but I was under the impression that there were springs and a pressure switch involved. You are literally just creating an end stop, plate to probe and your closing the circuit.

Pretty awesome right!

Just a correction on my part. Turns out the MAC version of Repetier DOES have the ability to save scripts. It’s on the GCode tab however and there are no buttons for it.