Mach3 errors need help

The G91 G28 Z0 is likely your culprit. G91 G28 tells mach3 (and lots of other controls as well) that you want to return the machine to it's zero point. This is the MACHINE zero point and not the part origin. Usually it's set to the extreme limits of the machine axis, but depending on how you have mach3 set up, it could be anywhere. Your frustration will be compounded if you don't have limit/home switches on your machine as it very well could change every time you start up mach3. The good news is that you can turn those commands off in the mach3 post processor in fusion360.

large


again, this is one of those things your simulator won't catch. So be careful out there!
 
oh, and to address your other question, G90 and G91 are brothers and are know as "modal" commands. Meaning that once a G90 (working in absolute coordinates) or a G91 (working in incremental units) is called up it remains active until the other command is called out. So by default your post is setting your units to be absolute in the very first line of code (what i call a safety block), but then the reference return command (G91 G28) switches to incremental. Your post is smart enough to know this so once the reference return is complete it switches back to a G90 for you.

The same is true for G00, G01, G02, and G03 commands. you'll never see two G0 callouts in a row or two G01's.

That make sense?
 
I hand edited the questionable lines out and it's running fine now.

cs900 said:
The G91 G28 Z0 is likely your culprit. G91 G28 tells mach3 (and lots of other controls as well) that you want to return the machine to it's zero point. This is the MACHINE zero point and not the part origin. Usually it's set to the extreme limits of the machine axis, but depending on how you have mach3 set up, it could be anywhere. Your frustration will be compounded if you don't have limit/home switches on your machine as it very well could change every time you start up mach3. The good news is that you can turn those commands off in the mach3 post processor in fusion360.

large


again, this is one of those things your simulator won't catch. So be careful out there!
Click to expand...

I was thinking that was the culprit so I edited it out. I looked in Fusion and it was on so I shut it off, will that be something I have to do every time I post a program or is there a way to set it to default to that setting. Also in fusion it always defaults to climb milling and I don't climb mill, is there a way to set some of those default parameters the way I want to, I haven't stumbled onto a way yet.

That is my learning method stumble and hit your head on the answer then it sinks in...

Yep the sim didn't catch this, fortunately the dry run without the tool did. The irritating part is it wasn't doing that last week when I was working on it so maybe that has to do with the machine 0 being different each time I turn the machine on, It doesn't have home or limit switches. Something I need to add.

Thanks
 
cs900 said:
oh, and to address your other question, G90 and G91 are brothers and are know as "modal" commands. Meaning that once a G90 (working in absolute coordinates) or a G91 (working in incremental units) is called up it remains active until the other command is called out. So by default your post is setting your units to be absolute in the very first line of code (what i call a safety block), but then the reference return command (G91 G28) switches to incremental. Your post is smart enough to know this so once the reference return is complete it switches back to a G90 for you.

The same is true for G00, G01, G02, and G03 commands. you'll never see two G0 callouts in a row or two G01's.

That make sense?
Click to expand...

Yes that makes sense, so the G91 that I left in line 10 is not necessary and the G90 in line 11 would still be necessary after the G91.1 in line 8?

Hopefully there is a way to edit the post so it puts out what I need and not all the extra stuff.
This is the hand edited version.
Capture4.JPG
 
I THINK it will remember to keep them off, but yes, it can be changed in the actual post processor as well. I'm happy to help out with that if need be. I think there is a way to save your cutting parameters so it defaults to whatever setting you want. I've only played with F360 a little so I can't say as if I know exactly how to do that, but it's something I'll be dealing with here in the near future.

Yeah, so depending on where you leave your machine will dictate where the machine origin is. You likely had you Z axis higher up last time you turned mach3 on. I can't recommend having home switches enough! there are so many cool things you can use them for to save yourself time.

While I'm thinking about this, in addition to the G91 G28 commands, you'll want to keep an eye out for G53 commands as well. I think the default mach3 post will post a G53 X0 Y0 at the very end oft he program. You may want to check as G53 does nearly the same thing as G91 G28 commands.

You do not need line 10; and if you delete line 10, you also will not need line 11. G90 is set in line 8. G91.1 is a different command than a regular G91 and will not effect the G90 callout. That said, your program will work fine as-is it's just a little "messy".
 
For info - most of the Fusion machining operations have the option of climb milling, conventional milling, or both.

What you are experiencing is called learning. Don't give up. You will eventually be very proficient at understanding and making gcode work for you.

I have a box of broken cutters on my work bench due to my mistakes and not understanding what the gcode is telling me. The box was filling up fast when I first started CNC machining. Now that I have a few years of experience under my belt it's been a while since I put a cutter in the box. You will get there too.
 
Ok I said it was running fine yesterday, I lied, it was hard to notice under the flood coolant but somehow in the changes I made to get it started it forgot the tool was 3/16" wide, it ran the tool path with the end mill centered on the contour it's cutting not offset by 1/2 the tool diameter.

When I started testing this code I ran the part successfully 3 or 4 times in MDF until I had it coming out correct, then I switch to steel and a whole new batch of problems SMH. It's times like this that I wished I drank. lol
 
I thought I did that.... I'll check. Yep I missed one. Had 5 out of 6 set to in computer.
 
You must log in or register to reply here.
Back
Top