Coding Problems, I,J,K errors

[dapoopta]

Trying to run on a HAAS TM1P. I attached the code. I keep getting that the radius of the circle isn't matching up. I am using solidcam as my processor, and have tried numerous post processors with no change in results. I have used NC plot and it gives the errors at the exact same position also. Thanks guys.
btw, if anyone has a quick fix for these please help! I need to get this done asap :-)

[jackson]

Have you looked into just using a G13 its much easer to wright that program seems way to long

[dapoopta]

the program was written with the SOLIDCAM software, which does it all for you. I am not familiar with g13.

[wganders]

Make sure the radius of the tool you're using isn't too big. If you're using cutter comp it will cause errors.

[HuFlungDung]

Its tough to tell by looking at the code without having the geometry to check against, but one setting which could be different between the machine and the post, might be that X has the option of being a diameter or radial value.

Try drawing up a simple square corner with a single corner fillet, toolpath it and post that and see if you can determine which setting is correct.

[dapoopta]

the tool is a 1/64" endmill. I looked at the solidworks file of it and it seems the fillets on the corners might have been causing the problem. I will stick it into solidcam tomorrow anad try, its time to go home now :-)

[wganders]

Note: always program the center of the tool for the tool path and leave the
radius value in the control set to zero (when using cutter comp). Just make sure you're using a tool with a smaller radius value than your smallest part radius feature. Works for me!

[SeymourDumore]

"""""

Note: always program the center of the tool for the tool path and leave the
radius value in the control set to zero (when using cutter comp).


""""


Good idea, that way dapoota would have a scrapped part instead of the control complaining that the tool is too big.

For what it's worth, no tool center programs will ever make it into my machines. Ever!

[SORCHEROR]

i have had that problem before and its always bad geometry or slines,did you draw the part or someone else,check the arcs and make sure they are good and trimmed correctly
its always with small arcs that ive noticed this problem

[dcoupar]

First, what alarm are you getting? Does it occur only on CW or only CCW arcs, or both? I don't remember if there's a "arc tolerance" parameter on the Haas, but there may be one.

It appears as if your post is outputting only 3 decimal places for X and Y, and 4 decimal places for I and J. This seems a bit odd, but may not be the problem. You might try configuring the post to output 4 places for X, Y, I and J. If that doesn't work, you could try outputting R instead of I and J. R is usually more forgiving, but the geometry may be off a couple of tenths. I personally have never had a problem with R's.

[Donkey Hotey]

Do you have probing? Did you use the tool presetter to setup the cutter diameters?

I had a problem that was driving me nuts. Cutter comp was on, the radius was .251 and was cut by a .250 endmill.

Well, the endmill touched off the presetter at .252 or something like that. It caused an error in that corner every time.

I went back to the original file and fattened up the radius to .260 and the problem went away.

[jackson]

Using a 7/16 end mill to mill a 2.03 pocket in alum.

G0G54G90X0Y0S6000M3
G43H1Z.1M8
G13G91Z-.8I.400K2.03Q.400L4D1F100.
G0Z.1

This stars with just a plat and steps it out and finishes it. I dont use cam so anything i can do th make my life easier.