Problem with a bit of g-code....

M

montejw

Plastic

Joined

Mar 1, 2003

Location

Bellingham, WA, US

• Mar 2, 2003

• #1

Hi,
New to the board and cnc. I have a Taig cnc mill that I just got running and I've been running some part programs I've found in different places. Here is a snippet of a part that seems to have a problem. I'm running Mach1 as my controller program. It is stopping on the G3 line and telling me that the starting and ending radii are different. Can anyone offer a bit of help on why this is happening? I need to study up on I and J moves, but haven't yet.

TIA,
Monte

G1Y.6
X-.49Y.49
X-.35
G3X-.49Y.35I.1J-.24
G1Y.49
X-.35

 

ARB

Titanium

Joined

Dec 7, 2002

Location

Granville,NY,USA

• Mar 2, 2003

• #2

Can we see a little more of the program starting a little sooner? Is your I and J set up absolute or incremental?

Take Care

ARB

 

M

montejw

Plastic

Joined

Mar 1, 2003

Location

Bellingham, WA, US

• Mar 2, 2003

• #3

ARB,
Here is the start of the program to a few lines past the problem spot. I think it's absolute, G90, right?

Thanks,
Monte

%
O0001
(CNCCUBE3.NC)
(TIME - 19:06 DATE - 04-02-02)
G0G40G49G80G17G90
T1M6
(TOOL - 01 DIA. - .2500)
(1/4 FLAT ENDMILL)
G0G54G90X-.1799Y.5649S4000M3
G43H1Z.1
G1Z0.F4.
X-.565Z-.0202
X.435Z-.0726
X-.565Z-.125
X-.615Y.6F8.
G2X-.6Y.615I.015J0.
G1X.6
G2X.615Y.6I0.J-.015
G1Y-.6
G2X.6Y-.615I-.015J0.
G1X-.6
G2X-.615Y-.6I0.J.015
G1Y.6
X-.49Y.49
X-.35
G3X-.49Y.35I.1J-.24
G1Y.49
X-.35
G2X-.25Y.51I.1J-.24
G1X.25
G2X.35Y.49I0.J-.26
G1X.49

 

M

montejw

Plastic

Joined

Mar 1, 2003

Location

Bellingham, WA, US

• Mar 2, 2003

• #4

Oh, and it's the G3 block after the X-.35 block.

Monte

 

M

montejw

Plastic

Joined

Mar 1, 2003

Location

Bellingham, WA, US

• Mar 2, 2003

• #5

I plotted the first G3 block in my cad program and it does seem to be incorrect. The next G2 block also stops Mach1. I guess I'll have to plot the points/arcs and hand edit the program to make it work. Unless someone can see something obvious that can easily be changed.

Monte

 

B

Bryan

Aluminum

Joined

Sep 24, 2002

• Mar 2, 2003

• #6

For what it's worth, I hand plotted that drawing in 3D CAD. It looks OK to me. Arc centers are incremental. You can download the drawing in dwg format here. I may have something wrong, but it seemed right when I double checked it. It is a strange tool path though.
Bryan

 

M

montejw

Plastic

Joined

Mar 1, 2003

Location

Bellingham, WA, US

• Mar 2, 2003

• #7

I thought arc centers could be either incremental or absolute. I plotted the block from an absolute point of view and it was incorrect. The start, end and center didn't work, I could only pick the start and center or end and center. If you plotted it from an incremental point of view and it worked I'll have to do that and see what it looks like.

Monte

 

B

Bryan

Aluminum

Joined

Sep 24, 2002

• Mar 2, 2003

• #8

I have no experience with that control, so I don't know if arc centers could be either absolute or incremental. I just see that the only way the G2's at the corners can work is if the arc centers are incremental, therefore the G3 has to be incremenatal as well. No need to replot the path, just download the one I did. I even reposted the code from BobCad with the drawing I made with incremental arc centers, and the code was exactly the same as you posted minus the formatting differences.

From BobCad starting at "X-.615Y.6F8."

X-0.615Y0.6
G02X-0.6Y0.615I0.015J0.
G01X0.6
G02X0.615Y0.6I0.J-0.015
G01Y-0.6
G02X0.6Y-0.615I-0.015J0.
G01X-0.6
G02X-0.615Y-0.6I0.J0.015
G01Y0.6
X-0.49Y0.49
X-0.35
G03X-0.49Y0.35I0.1J-0.24
G01Y0.49
X-0.35
G02X-0.25Y0.51I0.1J-0.24
G01X0.25
G02X0.35Y0.49I0.J-0.26
G01X0.49

I don't know why it won't run??

 

M

montejw

Plastic

Joined

Mar 1, 2003

Location

Bellingham, WA, US

• Mar 2, 2003

• #9

Bryan,
I found out that arc centers can be either incremental or absolute, depending on the control. All I had to do was switch my controller over to incremental for I J arc centers and it worked fine. According to a CNC handbook I have there isn't a standard, it's up to the control manufacturer. Mach1 has a switch so I can run it either way.

I guess I have a 50/50 chance of getting the setting right for programs that I don't know how they were programed.

Monte

 

B

Bryan

Aluminum

Joined

Sep 24, 2002

• Mar 2, 2003

• #10

That's cool. Here is my experience with absolute and incremental arc centers: All of the mentioned machines, I either run or program for.
On a 8000 G&L, if you are in G90, arc centers are absolute. If you are in G91, arc centers are incremental.
On a 840C and 850M Siemens, arc centers are based on a parameter setting, so how ever you set up the control initially is the way you continue to program it.
On a Robotool control, I can freely select absolute or incremental arc centers. G75 is absoulute and G74 is incremental. I like this option the best of any of the controls mentioned.

 

B

Bryan

Aluminum

Joined

Sep 24, 2002

• Mar 9, 2003

• #11

Monte,
I just downloaded the manual for your control from the thread you posted to with the info to Mach1. It says you can use R instead of I and J. I like that better than I and J. With R you never have to worry about incremental or absolute arc centers. It is also in my opinion, easier to verify the program with R when you are doing semi-circles. For example, the code you were originally having problems with, if it were programmed with R instead of I and J, it would look like this:

G1Y0.6
X-.49Y.49
X-.35
G3X-.49Y.35R.26
G1Y.49
X-.35
G2X-.25Y.51R.26
G1X.25
G2X.35Y.49R.26
G1X.49

Bryan

 

M

montejw

Plastic

Joined

Mar 1, 2003

Location

Bellingham, WA, US

• Mar 9, 2003

• #12

Hi Bryan,
Yeah, R is easier than I and J. I would probably program R arcs if I can. I'm still going through the 'demo' state trying to decide on a CAM program. Currently looking at Dolphin CAD/CAM.

The program was something I downloaded and from a votech teacher's web site. It works as is (as long as your controller is setup for incremental arc centers) and I learned something from it, which was the goal.

Monte