Problem- Strange behaviour with G17/G18 in Maho Mill

[jeuhrn]

I don't know wether my problem is bug or feature, and if so if it pertains to my machine only or G-code in general but here it is:

I'm working in a Maho MH 600 which has a vertical spindle but is by default operating in G18. In order to solve a specific problem i have to do a G2 in G17. (To mill a R4.3 groove on the upwards face of a piece). Meaning when I execute a G2 in G17 the tool moves in Z (vertical) direction, which is Y on this particular machine. (sigh.)

What happens is that my program runs fine when I use a tool with length offset 0, but if it _does_ have a length offset my coordinates change in the line where I switch to G17.
There's no motion when it does G17, just the coordinates on the screen offset some, and my G2 instruction gets a bigger radius (according to tool length offset) and starts working in G0 speed.
The part about rapid feeding should be impossible in a G2 instruction according to my common sense, but that is what it does.
The result was 10mm of mill crushed into my workpiece.

I spent hours identifying the problem, and when I did I tried changing the tool offset to 100mm and running the program.
The G2 instruction wanted to circumfer the whole machine itself I think, but it stopped itself with the nice error message (paraphrased) "movement faster than rapid".

Has anyone ever seen this behaviour before?
Let me know if it was unclear or if you need any more info to provide some input.

[JWK42]

jeuhrn
I have been programming Maho 600 for a few years now. Can you post your drawing or your code that is giving the problem and I'll check it out in the morning. I think we are PM - 6 hrs so it 3:40 PM here and time to call it a day.

Jerry

[jeuhrn]

The drawing is probably "top secret", but I can post the code.

N1 G52 S2500 T1 M66
N2 G0 Y20 M13
N3 GO X0 Z0 
N4 G0 Y1 Z-1.3
N5 G1 Y-3 F150
N6 G17
N7 G2 Y-3 Z1.3 J-3 K0
N8 G92 X-0.22
N9 G14 J775 N1=4 N2=8
N10 G0 Y10
N11 M30

This makes a half circle in the 'seen from the side' plane, and you get a R4.3 groove with a R3 ballnose mill, and then it moves X-.22mm for the next iteration.

I've never been on a mill before where Y-axis is Z and vice versa, and X traverses + in the 'wrong' direction, but I'll assume all Maho 600's are the same (if not you are bound to be confused by this code).

So basically this works fine as long as tool length is 0 (which I always keep in T1), but when I use a different tool with length offset, G17 will shift the coordinates in both Y and Z axis but not X, and the following G2 goes haywire. The larger the tool length offset the crazier it gets.

If you are gonna try this I advice you to keep a good distance from the table just to be safe.

[JWK42]

Remember a Maho MH600 is commisioned as a Hortzontal Mill so the X is left and right and the Y is up and down and the Z axis is the Horizontal axis so it defaults to G17 on startup. G17 applies tool length comp to the Z axis or horizontal Axis. I am assuming you are milling this part with the swing around head which makes a Vertical Mill or G18 unfortunely this means the tool length comp is applied to the Y axis. But you must call G18 to make it switch to the Y axis
So when you switch to G17 you transfer what ever is in your tool 1 table from
the Y(G18) to the Z (G17) axis. In my program I am switching to G19 so tool length comp would be applied to the X(G19) axis. That is why I would use Zero tool length comp
I also think you are actually machining your radius around the X Axis since you
incrementing along the X between passes. Therefore you need to use G19 to Circle around the X axis.
We always use a G93 Absolute Zero Offest to establish the program Zero Point.
If you touch off the tip of your tool at the point on your part you want for
Part Zero and enter those coordinates in the G93 line in your program.
then set tool 1 length to zero in the tool table.
I would try the code below it is not much different than yours.
I hope this helps. I love our Maho Mills but it drives you crazy when you start programming "Normal Mills". We only have 1 Maho left.
Our Maho is busy so I won't have a chance to test this so remember "Rapid Over Ride" and "Cut Air" first.
Edit
Because the rapids always go home on the measuring axis first, in this case X axis, I would add a line N85 to rapid in the Y first the Z.


I also would have changed line 90 to--

N90 G91 X-.22
N95 G90
Rather than the G92 X shift.

N10 G52 S2500
N15 G18 T1 M66
N20 G93 X11.803 Y3.606 Z11.677 (ABSOLUTE ZERO OFFSET)
N30 G0 Y20 M13
N40 G0 X0 Z0
N50 G0 Y1 Z-1.3
N60 G1 Y-3 F150
N70 G19
N80 G2 Y-3 Z1.3 J-3 K0
N85 G0 Y1 (ADDED THIS LINE)
N90 G92 X-0.22
N100 G14 J775 N1=50 N2=90
N110 G18 G0 Y10
N110 M30



Your Code
N1 G52 S2500 T1 M66
N2 G0 Y20 M13
N3 G0 X0 Z0
N4 G0 Y1 Z-1.3
N5 G1 Y-3 F150
N6 G17
N7 G2 Y-3 Z1.3 J-3 K0
N8 G92 X-0.22
N9 G14 J775 N1=4 N2=8
N10 G0 Y10
N11 M30

[jeuhrn]

This one has a 'swing-around' head yes, but it defaults to G18 when starting up.

My workaround was to call T1 with 0 length offset in the program but set the zero point in G54 to compensate for the length, although G93 would have worked just as well. And it literally took me hours to figure out how to get this machine to store G54-G59, which the manual provided about 0 information on. I just started working here a few months ago, and the guy who ran this machine before has moved on, so now I'm the 'expert'.

What I'm curious about though is how it can move rapidly in G2, isn't G2 supposed to always run in the feed from the previous G1?

[JWK42]

Your machine is commisioned differently than normal. This may have been done as a new machine or on rebuild. So the G19, G18 and G17 may apply to diffferent axis than ours. We use G54-G59 very rarely because our first trainer in 1984 prefered G93 Absolute Zero Shift and old habits are hard to break. We use G54-G59 on all our Haas Mills.

I wonder if changing to G17 causes the Modal Feed Rate to be lost. Try putting a feed rate in the G2 line. Your F150 scared me until I rememered you are in MM mode not Inch

[jeuhrn]

I did have a feed rate in the G2, but it doesn't affect anything. Also it's faster than G0, which is why it triggered the "movement faster than rapid" error when it tried to go in a really big circle.

I'll take your word on it being commisioned different than normal, and that probably has something to do with it.
I think I'll just have to make a mental note to always keep tool length 0 when switching planes, or experiment and figure out a way to reset the correct zero point after G17/G18/G19.

[JWK42]

Now I'm stumped!!
Does G2 feed correctly in a different program?
Can you use a R word to swing your radius instead of J & K?
I think you would get an illegal format it you had an 'O' instead of Zero in your code. I noticed an 'O' in line N3. I assume you hand typed those lines into this thread. I am still not sure if I have a good picture of what your part looks like. We have used your method of multiple passes over a profile many times. If you would PM me your E-Mail I will send you mine so you can send a jpeg picture of a small portion of your print, if you are allowed to.
I would like to try to create the code and test it on our machine when it opens up.

[stevo1]

You can use the R to swing a radius as well. The only thing I see different in the G2 line that I have is an X value. Might need this so it know what it is swinging around. Try G2 X0 Y-3 Z1.3 J-3 K0 you can probaly get rid of the K.

I had the same problem on the 5 axis I have been working on. Once I instated the tool offset it went to the wrong place. The G17 and G18 were set up weird. Try using the G17. I also had a problem if I sent the machine home with a G28G53Z0 then tried to move from there. I think it would cancel my tool offset but the tool number stayed active?????

Stevo