Need help with circular / helical gcode errors

[jsheerin]

Hi,
I'm trying to get going with my router I just finished. I am using visual mill 6 to generate gcode. I'm currently trying to route a hole. I have visual mill set to ramp the cutter into the hole as opposed to just plunging. Using the mach3-inch post in visual mill, I get code like this:
G17
G03Z-0.1050I10.1700J1.3400K0.1050

And mach3 tells me: k word given for arc in xy plane

I've searched here and on the visual mill forum with no real luck. I did find a suggestion to use the mach2 post in visual mill, but that just produced a bunch of other problems. However it did not produce a circular interpolation command with a k word in it, so I at least got to play with my router for a while before I realized it wasn't cutting what I'd drawn...

So from more reading, it seems that mach3 interprets g2/g3 commands to only need I and or J values with a Z value to create the lead of the helix. It also seems to want I / J to be I/K or J/K if the g2/g3 command is in a plane other than XY. But visual mill wants to output K values for the lead of a helix and Q values for leads of a spiral. If I'm doing hole pocketing, these K and Q values are always the same but really there should be a Z value that keeps changing to reflect drilling deeper? I get this from reading page 121 in the Mach3Mill pdf (page 10-17). So from this plus some other oddities I just found in visual mill, I conclude the visual mill post for mach3 is wrong.

This is just me thinking through this problem out loud, but if anyone has any suggestions or experience, I'd love to hear them. I think I'll be emailing visual mill's support people now.

[tobyaxis]

Assuming Mach3 is based on a Fanuc Control your G-Code should read close to this but with different coordinates.

N1(EMILL 1/2D)
T1M6
G90G54G40G0G17G0X0Y0S1000M3
G43Z.1H1M8
G1Z.025F30.
G41G1Y-.25F10.
G3X0Y-.25Z-.125J.25
X0Y-.25Z-.25J.25
X0Y-.25Z-.375J.25
X0Y-.25Z-.5J.25
G40G1Y0
G0Z1.M9
M5
G91G28Z0
M1

This program goes to X0Y0 then .025 above the part surface. calls cutter comp in the y axis. After that it Interpolates in all 3 axis at Z-.125 , Z-.25, Z-.375, then Z-.5 in a Helical Motion.

See pic below.

The K in you code is parallel axis to Z, so I don't think it belongs there, but I could be wrong because this is a Mach control, not Fanuc.

[ger21]

A G2 or G3 can not have a K in it when using G17. You're going to need to fix the post. What exactly was wrong with the Mach3 post?

[jsheerin]

Thanks guys. I appreciate the sanity check. Yes, from reading the mach3 manual, I think your code should work Toby. My issue is how to get visual mill to generate that now. I didn't buy it so I could write code by hand. I also didn't buy it so I could spend hours screwing around editing an incorrect post configuration (for what seems to me to be a rather basic issue). The mach3 post generates the K in the G2/G3 commands, so that is what is wrong, to answer Gerry. Maybe that was not clear in my ramblings above. But beyond that, I'm not sure from looking at their post editor as to how to correct that issue. I've emailed mechsoft asking for a fix, so hopefully they will take care of me.

[mactec54]

Hi jsheerin

Tobyaxis has the right idea but here is a easyer way to do it & not so messy

G2X0.Y.3125Z-.15I-.3125F12.
Z-.35J-.3125
Z-.55J-.3125
Z-.75J-.3125
J-.3125

See attached txt file you should be able to run on you machine
It is a 1inch hole X0Y0 with a .375 cutter speeds & feeds you can ajust for your machine it also does a ark off at the end of the cut

[tobyaxis]

Originally Posted by mactec54 Hi jsheerin Tobyaxis has the right idea but here is a easyer way to do it & not so messy G2X0.Y.3125Z-.15I-.3125F12. Z-.35J-.3125 Z-.55J-.3125 Z-.75J-.3125 J-.3125 See attached txt file you should be able to run on you machine It is a 1inch hole X0Y0 with a .375 cutter speeds & feeds you can ajust for your machine it also does a ark off at the end of the cut

I like your shorter code, lol. I was unable to do it that way because the control always had a fit with alarms. It wanted to see all 4 designations in every sequence block for some strange reason. LOL, it was a new machine control too. Oh well.

[mactec54]

Hi tobyaxis

What controls do you have it may be just a simple change some were to make it run I have run it on 3 different controls without any problems

Save the txt file & try it on your machine

[tobyaxis]

Originally Posted by mactec54 Hi tobyaxis What controls do you have it may be just a simple change some were to make it run I have run it on 3 different controls without any problems Save the txt file & try it on your machine

Thanks but I no longer work for that employer.

Honestly your method saves memory but as long as it works for thread milling and helical entry, I'm happy.

[jsheerin]

Just to update, Mecsoft helped me out and mactec's code is now what I'm putting out. Unfortunately, it forces me (as far as I can tell so far) to cut the OD of the hole first and then go back and clean up the middle at full depth. But I'd rather cut into the middle of the hole with full cutter engagement and then clean up the outside perimeter of the hole with a lighter cut.

[tobyaxis]

Originally Posted by jsheerin Just to update, Mecsoft helped me out and mactec's code is now what I'm putting out. Unfortunately, it forces me (as far as I can tell so far) to cut the OD of the hole first and then go back and clean up the middle at full depth. But I'd rather cut into the middle of the hole with full cutter engagement and then clean up the outside perimeter of the hole with a lighter cut.

There might be an option to start at the center and work toward the outside. This means you will have to set a step over limit.

There should be something in the Tool Path Parameters. Give it a look see.

[jsheerin]

Well, I assumed the default operation would be to start at the center. What tech support suggested was to use the feed in setup screen to essentially create the feature. Playing with it some more, I found that it will generate good code if I set the feed in helix diameter smaller. However, it seems (from an admittedly fast look) that it does not correctly generate paths for clean up cuts at various Z levels. Iow, it will feed down in a helix to the bottom of the hole and then clean up the outside diameter of the hole (as I wanted). It just can't do that in various Z steps without me setting up multiple cutting operations to do it.

[tobyaxis]

This type of step down is better for deep holes. It allows for better finishes and lighter loads on your tool.

Play around with it some more and see what parameters do what.