[Matt Clara]

I've searched around and I can't find exactly what I'm looking for, so I thought I'd just ask. I've cut three or four things now, including a couple radius dishes for building guitars with, which came out well, but I'm getting ready to try some 3D carving and there's one thing that bothers me about how I go about this and I figure I must be doing something not quite right here. When I open the G code in Mach3 and then touch off the work piece and zero the system/regen the toolpath, I'm ready to cut, but my router bit is still touching the work piece and when I turn it on it'll leave a mark there. Now, if that spot is going to be cut in the course of the operation, no big deal, but if it's not, then I have a mark I need to deal with. Am I supposed to raise the zed before telling Mach to commence the cutting operation? Would soft limits interfere, or are those only in relation to the machine coordinates, and not the work coordinates established when the work piece is touched and the coordinates zeroed?

I did try raising the zed before cutting once, but my softlimits were turned off. Problem is that when cutting commenced, the zed plunged quite a bit deeper than it should have and I had to stop operations and re-zero. I've tweaked my machine setup in Mach quite a bit since then, but since I don't really know why it did that before, I'm not at all assured it won't do it again...

Thanks!

[Bert.C]

You can move the z axis up before you press cycle start. I think 99.9% of operators would to be fair. Also soft limits shouldnt interfere with the cutting unless the part is too big for the machine to cut.

As for the plunge. Why not try zeroing the machine with the z axis higher than the work piece and see if it plunges to below where you zeroed it just as a test?

Sent from my GT-N7100 using Tapatalk

[CarveOne]

In the software that you use to generate the gcode there is usually a material setup screen that allows you to set a rapid Z gap above the material and also a plunge gap. These are used to set gaps above the material to clear any clamps that the cutter may run into. I don't use clamps, so I have both settings at 0.125" above the top surface of the material to cut down on the overall cut time.

These settings may be what you are missing. They raise the cutter when the cutter needs to move to another coordinate and start cutting.

[bhurts]

Post a bit of the code your running. Just the first 50 lines or so. That will tell us what the machine is going to do when you hit start. You should move the z up off your part atleast to rapid height before running anything.

Ben

[Devastator]

Ideally, your code should retract the Z to the rapid height before starting the router. Not sure what CAM program you are using, but that should be standard protocol. It should not start the router @ Z zero.

If you are manually turning on the router via a switch, yeah, don't do that until you jog the z away from the piece, then start your run.

Once you zero, the machine knows where it is from there, so you can move it wherever you need to get it away from the piece before starting the router, then hit start.

So do your zero procedure, jog the z up, start your router, then start your file, no more divot.

[Matt Clara]

Thanks guys. Here's a short one for cutting a soundhole and routing a channel around it for a rosette inlay. I add the M3/M5 myself, so I'm guessing I should be adding it after the z raises to the rapid clearance height...?


M3
N110G00G20G17G90G40G49G80
N120G70G91.1
N130T1M06
N140 (End Mill {0.25 inch})
N150G00G43Z0.8000H1
N160S12000M03
N170(Toolpath:- Profile 1)
N180()
N190G94
N200X0.0000Y0.0000F100.0
N210G00X0.0000Y1.2632Z0.2000
N220G1Z-0.0400F30.0
N230G2X-1.3750Y2.6382I0.0000J1.3750F100.0
N240G2X0.0000Y4.0132I1.3750J0.0000
N250G2X1.3750Y2.6382I0.0000J-1.3750
N260G2X0.0000Y1.2632I-1.3750J0.0000
N270G00Z0.2000
N280S12000M03
(Profile 2)
()
N310G00X0.0000Y1.6382Z0.2000
N320G1Z-0.1000F30.0
N330G3X1.0000Y2.6382I0.0000J1.0000F100.0
N340G3X0.0000Y3.6382I-1.0000J0.0000
N350G3X-1.0000Y2.6382I0.0000J-1.0000
N360G3X0.0000Y1.6382I1.0000J0.0000
N370G00Z0.2000
N380G00Z0.8000
N390G00X0.0000Y0.0000
N400M09
N410M30
M5
%

[Devastator]

I add the M3/M5 myself, so I'm guessing I should be adding it after the z raises to the rapid clearance height...?

There is already an M3 in the file at the start right after the RPM (S12000). Ideally it should have a Z command away from the part, then the M3, then a dwell (G04) in milliseconds for the router to spool up, then the file run.

Looks like there is already a retract command before the M3 to Z.80, but since you've added in your own M3 at the start of the file, you are your own worst enemy.

You might just try deleting your M3 at the top.

[Matt Clara]

Thanks, that worked! Now, one more time, if I zero the zed and then raise it manually, can I just hit start cycle and Mach will know where everything is and start the cutting accordingly? I'm nervous to try it after the last time when it plunged 1/4" ball nose mill nearly a half inch into the mdf. Does that sound as though I might have something set up wrong? If I don't raise and then start, everything goes according to plan, but as I don't have a tool changer, so I tend to run one tool path at a time, raise the zed when it's done, change bits, load the new z code, rezero the z axis, regen the tool path, and then hit cycle start. If the tools are the same length, which they are in many cases (the ones with the tool change rings on them), it would be nice to just raise it, change it, load the g code and hit cycle start...

[Devastator]

Thanks, that worked! Now, one more time, if I zero the zed and then raise it manually, can I just hit start cycle and Mach will know where everything is and start the cutting accordingly?

Yes. I usually do this the first time I run a file just in case.

I'm nervous to try it after the last time when it plunged 1/4" ball nose mill nearly a half inch into the mdf. Does that sound as though I might have something set up wrong?

Yes, it sounds like something in your set up was wrong.

If I don't raise and then start, everything goes according to plan, but as I don't have a tool changer, so I tend to run one tool path at a time, raise the zed when it's done, change bits, load the new z code, rezero the z axis, regen the tool path, and then hit cycle start. If the tools are the same length, which they are in many cases (the ones with the tool change rings on them), it would be nice to just raise it, change it, load the g code and hit cycle start...

You can do that, but I never personally trust those rings 100 percent. What I do is write a tool change script where the tool change goes. I have it bring the router up front and center and then shut off where I can reach it for easy changing, then re-zero, then hit start. I only use one file, but I add my tool change script manually every where in the file I need to change the tool or add hold down screws. That way I don't have to load multiple files every time I change tools.

[Matt Clara]

So, I suppose I'm going to have to learn this G Code thing and write my own script, eh. ********.

Thanks for your help, btw. I appreciate it.

[ger21]

What CAM software are you using? Your CAM software should add M3/M5, and M6 for tool changes.
With Mach3, you can get the Big Tx Mach Blue or my 2010 Screenset, which automates the zeroing of the Z axis after tool changes.

When I have multiple tools, when the g-code gets to M6, the machine goes to my tool chane position and stops. I change the tool, and click Cycle Start. Mach3 automatically measures the new tool, and continues cutting.

[Devastator]

So, I suppose I'm going to have to learn this G Code thing and write my own script, eh. ********.

Thanks for your help, btw. I appreciate it.

If you just watch the screen as it runs your file you'll learn a bit. I used the MDI screen a lot when I first set mine up to play around with moving it around. You type a G command in the box and see if it does what you thought it would. After awhile you can look at the code in your file and tell what it means. Good for troubleshooting.

Like ger21 says, you can just get certain screensets that will have auto zero scripts built in. I tried those at first and broke some bits, so I do it by hand now. I'll probably revisit it at some point. I'll probably be able to tell what I was doing wrong now that I have some time under my belt.

[nytwin1]

Originally Posted by Ger 21

What CAM software are you using? Your CAM software should add M3/M5, and M6 for tool changes.
With Mach3, you can get the Big Tx Mach Blue or my 2010 Screenset, which automates the zeroing of the Z axis after tool changes.

When I have multiple tools, when the g-code gets to M6, the machine goes to my tool chane position and stops. I change the tool, and click Cycle Start. Mach3 automatically measures the new tool, and continues cutting.

I got Big Tex's new script and have a problem with it. I followed the instructions in the video. I the initial setup button works as shown.The zero tool setup button seems to be caught in almost a loop. It never would go back to the work piece, but ends up tripping my limit switch in zed. Any idea why this might be happening?