Need Help!- HAAS Radius error

[QMI2007]

I am using Mastercam X2 and have an issue when I post a simple 2D program out to my HAAS. It uses an R command for G2/G3 moves instead of I/J which is how it's always been. I have had problems since I downloaded X2-MR1. If there are two arcs tangent to each other(for instance if you were to mill the outside profile of the Mastercard logo) instead of going around the outside of both circles it will make its own arc connecting the end point of the first arc to the end point of the second arc in the shortest distance possible which instead of following the correct contour. Is there an arc tolerance or some other setting in the HAAS control that could eliminate this issue?

[CNCRim]

post a design file with toolpath we might see something. You can edit the post to output R instead I/J.

[Geof]

It could be that the arc you need goes past 180 degrees. When you are using R for G02/G03 and the arc is larger than 180 degrees the R value has to be negative; if it is less than 180 degrees it is positive.

[Donkey Hotey]

This really belongs in the Mastercam forum.

I had a similar problem last night. I was trying to clear a round pocket in MC X. When it posted, the command was a positive R value and caused an error on the Haas.

I haven't had time to experiment with it yet to find out why it posted that for one pocket but not the others.

Where did you get the post? Has it been modified?

[QMI2007]

I dont think this is a Mastercam issue. Although it could be. The way I do things is the same as it always has been, these types of parts are new to this company though. I am less framiliar with Haas than I am with MCX that is why I feel there is some type of setting that is being overlooked and I dont have anyone here that really knows the machines either.
I have several Haas post processors, some that I have used for years at other companies, some were here when I started, some from colleagues which have always been fine. This problem has only begun occuring since running MCX2 MR1 in certain situations when posting with an R command. 85% of the time there is no problem but it seems to be popping up more on me. I did play around with it when it was in the machine, frustration set in and my only solution was re-posting certain toolpaths using I/J command.
For those who have had similar issues: I just had another one come up this morning. Helical milling a counterbore, and the last pass doesnt go around at final depth, it just reaches final depth and retracts out, thus leaving a spiral in the bottom of the hole??????

[Geof]

Originally Posted by QMI2007 ..... Helical milling a counterbore, and the last pass doesnt go around at final depth, it just reaches final depth and retracts out, thus leaving a spiral in the bottom of the hole??????

Show us the code.

I have made a mistake in a program that gave me this result. This is an example of the code:


G91 G03 I0. J-.4 Z-.1 F50. L4
This line goes around four times incrementing down 0.1 per circle. But there is a ramp at the bottom of the hole so you need to go around once more to take that out.

Instead of typing the complete line I copy this one using the editor and change the G91 to a G90 to get:

G90 G03 Io. J-.4 Z-.1 F50. L4

I do not want to go around four times so I take the L4 away:

G90 G03 I0. J-.4 Z-.1 F50.

And run the program....and wonder why I still have a ramp at the bottom of the hole???

I forgot to take out the Z-.1 so once I have gone back to absolute the Z moves up to -.1 absolute on the last circle.

When I find it I feel a bit silly.

[QMI2007]

here is the code that did not leave the c'bore flat at the bottom:


Z5.37
G01 Z5.27 F40.
G41 X-4.165
G03 X-4.415 Z5.245 R.125
X-4.165 Z5.22 R.125
X-4.3362 Y.8912 Z5.2045 R.125
X-4.165 Y.775 R.125
X-4.3583 Y.8797 R.125
G01 G40 X-4.29 Y.775
G00 Z9.

when I post it with I/J it works fine though????

[Haas_Apps]

I just put this program in MetaCut and it shows that there is a problem with the G-code. See attachment.

[HuFlungDung]

My 1996 Haas VF3 may have some bug in the software, but the other day I was performing a clean circle operation in 10 holes in sequence. The operation consisted of two complete circles, no tool comp involved.

So it did the first three holes normally, then on the 4th hole it seemed to skip one of the circles, did a few more holes, then same thing again.

Only thing I had changed lately was to change my post output to permit complete circles to be cut with one command. So, I changed it back to half circle max per command, and then it worked fine.

I was using IJ arc centers, not R.

[SeymourDumore]

First of all, that code snippet without the starting X and Y coords is useless as none of the backp[lotters can figure out where the paths start from.
Also, you seem to have the modal coords turned off in MCX. It isn't a problem for Haas but it is a problem for trying to figure out where your problem is.
One thing, the Haas is doing circles the very same way Pre or Post MCX, suggesting that the problem is in your post or how MCX handles the post. Pointing the finger at the control when your software has changed is not logical.
Anyway, as Geof said, R is positive for arcs less than 180 deg, and negative for above but not more than 359 degree. If the arc is a full circle (which the Haas can do just fine) you MUST use I and J, you can even omit the X and Y coords.
IOW the following code will make a 1" radius circle with it's center at 0,0:

G01 X0 Y.5
G02 I0 J-.5

Anyway, post the whole code and perhaps add the modal coords as well because the above snippet will make only one full circle and a bunch of small arcs within the circle.

[Geof]

Originally Posted by SeymourDumore ..... the above snippet will make only one full circle and a bunch of small arcs within the circle.

I did put in an arbitrary start position and ran it in a Haas simulator; it did the two semicircles to complete the full circle than gave a radius error and would not go further so I didn't go any further.