"Circle Not Congruent" ...What??

Hello;

So I'm having a problem with my EnRoute 4. It seems like whenever I use my computer on the CNC router at my work, it stops and gives me this message:

http://i58.photobucket.com/albums/g2...tCongruent.jpg


I have no idea what the machine is talking about. The coding looks fine to me; there's nothing all too weird there. I didn't find anything in the manual for an error code like this; I looked it up on Google and found no answer. I checked the parameters in my EnRoute and compared them to the other computer at work (running EnRoute 3) and they all match. So I have no idea what to do.

Does anyone have any idea what this means? It's driving me crazy, and it's been holding me back from some jobs. The router will be in the middle of cutting and then just stop--it freezes, but the spindle is still going, while that error comes up on the screen. I have no clue what would make it do this, and I'm just hoping that someone else would know what to do.

Might be that the arc centers are incorrect in relation to the start and end points of the movement. It only takes an error of .0001" to cause this problem on some unforgiving controllers.

If you want to zip up your nc text file and post it here, someone could run it through a backplot to see how it looks.

Do you have your arc centers set as incremental or absolute coordinates and what does the controller require?

Quote:

---

Originally Posted by HuFlungDung

Might be that the arc centers are incorrect in relation to the start and end points of the movement. It only takes an error of .0001" to cause this problem on some unforgiving controllers.

If you want to zip up your nc text file and post it here, someone could run it through a backplot to see how it looks.

Do you have your arc centers set as incremental or absolute coordinates and what does the controller require?

---

I had a feeling that it was coming out of the computer wrong. How do I go and look to see if it's incremental or absolute, and what the controller requires?

Sorry, I'm sort of a noob.

And here's the file:

G1 X22.1396 Y3.9415 Z0.6830

Your first line of code (before the highlighted line) positions the x & y. This is your initial start position. This will be the start point of an arc, and is on the arc.

G3 X21.9410 Y3.5897 I 35.1932 J-3.6572

This highlighted line tells the machine that the center of rotation is (X current position +35.1932, Y current position -3.6572) or (57.3328, .2843)
It also instructs the controller to CCW arc to (21.9410,3.5897).

The problem is, this new point is not on the arc defined by the first line and the center of rotation. If it was, it would have the same distance from center as the first point. SQR((x-xc)^2+(y-yc)^2).

You're using absolute coordinates for the I & J, and the controller is expecting incremental coordinates.

Quote:

---

Originally Posted by Eurisko

G1 X22.1396 Y3.9415 Z0.6830

Your first line of code (before the highlighted line) positions the x & y. This is your initial start position. This will be the start point of an arc, and is on the arc.

G3 X21.9410 Y3.5897 I 35.1932 J-3.6572

This highlighted line tells the machine that the center of rotation is (X current position +35.1932, Y current position -3.6572) or (57.3328, .2843)
It also instructs the controller to CCW arc to (21.9410,3.5897).

The problem is, this new point is not on the arc defined by the first line and the center of rotation. If it was, it would have the same distance from center as the first point. SQR((x-xc)^2+(y-yc)^2).

You're using absolute coordinates for the I & J, and the controller is expecting incremental coordinates.

---

So what would the correct coding look like? I'm trying to figure this out, but I'm having a hard time understanding this at the moment; I'm fried from work.

And I've actually been using absolute coordinates for a while on this machine, but lately it's been acting up. I don't understand why. It's like my computer keeps doing the math wrong.

Every industrial CNC machine I've seen uses incremental I&J to specify an arc center. I'm sure that there is a machine parameter that would allow the use of absolute I&J, but let's stick with incremental for now.

The first line is unchanged.

G1 X22.1396 Y3.9415 Z0.6830

The second line becomes:

G3 X21.9410 Y3.5897 I 13.0536 J-7.5987

The I parameter tells the controller that the arc center X is 13.0536 inches from the current X position and the J parameter says that the arc center Y is -7.5987 inches from the current Y position .

Even though the X,Y, and Z moves are absolute (G90), the I & J parameters are incremental. Just offsets from the current (X,Y) position.

You can calculate the arc radius directly from the incremental I,J values:
r=SQRT((I^2)+(J^2))
r=15.1042 (to 4 decimal places)

We know that the initial point is the start point of an arc. How about the 2nd point, X21.9410 Y3.5897 ? Does it lie on an arc centered at (X=22.1396 + 13.0536, Y=3.9415 - 7.5987 ) ? Calculate the distance from the 2nd point to the arc center:

r1=SQRT( (21.941-(22.1396+13.0536))^2 + (3.5897-(3.9415-7.5987))^2 )

r1=15.1042 (to 4 decimal places)

The two radii match. The 2nd point is ON the arc, and your controller shouldn't complain. Whew! I'm done.

So basically, the controller SHOULDN'T complain...but it is?

And thank you for doing all that math for me. Lol.

HI everyone,

Long time reader, first time poster! Having done woodworking in the past, I thought it would be fantastic to branch out and buy me a table-top CNC router. It came from China with very little instructions.

I have purchased some programs for digitizing and downloaded some trial programs for such things as 3D molding and such and have had a little success at doing some projects, but I cannot get a perfect circle to come-out of this thing to save my life!!!

I know that there is a lot to learn and I have learned lots already by reading the boards, but can someone tell me is there some trick to get it to cut a circle. I have an older version of Mach 3 that I am using, and settings I should know about? Thank you in advance.

JB

Quote:

---

Originally Posted by JMBPromotions

HI everyone,

Long time reader, first time poster! Having done woodworking in the past, I thought it would be fantastic to branch out and buy me a table-top CNC router. It came from China with very little instructions.

I have purchased some programs for digitizing and downloaded some trial programs for such things as 3D molding and such and have had a little success at doing some projects, but I cannot get a perfect circle to come-out of this thing to save my life!!!

I know that there is a lot to learn and I have learned lots already by reading the boards, but can someone tell me is there some trick to get it to cut a circle. I have an older version of Mach 3 that I am using, and settings I should know about? Thank you in advance.

JB

---

If I were you I would go to the Artsoft(Mach) support forum and ask the question there. I would bet it has to do with your motor tuning in the x and y axis

Mike

Thanks Mike. I reread the installation and whatever info I could find. Now it seems to be doing better. But I have a long way to go before I am actually doing what I want.

I've been having this problem recently and found that the solution was to change the machine set-up to generate code for arc segments from the radius and use a relative center.