The never-ending saga of the Hurco that's "ready to make parts"

E

ecdez

Forum Guest
Register Today
I've been chasing gremlins on this machine for two weeks and finally got to cut some metal today only to find a new gremlin.


I have some code to cut a circle 1.339" in diameter (inside cut). Here's the code.

%
N10 G70 G17
N20 G40 G90
N30 S1000
N40 T1 M06
N50 G00 Z0.5
N60 S1000 M03
N70 X1.8954 Y0.4149
N80 Z0.0197
N90 G01 Z-0.06 F4

(All is good until here)

N100 G02 X1.3992 Y1.4519 I-0.2226 J0.5307 F12.0
N110 X1.6702 Y1.5211 I0.2736 J-0.5064
N120 X1.8954 Y0.4149 I0.0026 J-0.5755

(Back to good again)

N130 G00 Z0.5
N140 M05
N150 M02
E




I have two problems with it and both are equally disturbing.

#1 - circle comes out to just over 3.75" in diameter.

#2 - circle has a small (1/2" x 1/2") pac-man mouth in the 2 o-clock position


Machine is a Hurco with Ultimax. Code comes up on the display after being dripped in and it's the same as shown above. Double checked that everything is in inches. Generated the code twice with the same results.



Anyone have any ideas?
 
Re: Code issue, please help. This stopped being fun a few days ago.

Check to see if the circle center is in absolute or incremental mode, it looks like it's incremental. Are you using a CAM program or are you generating this code on the machine.

EDIT:

I loaded your G-code in to my cam program, and yup, it has a PacMan mouth looking feature. Check your drawing to make sure there are no hidden lines or artifacts hiding. If you will post the hole center location from 0,0 and tool size, I'll run it through my CAM program and correct your G-code.
 
Last edited:
Re: Code issue, please help. This stopped being fun a few days ago.

I am still new, but was checking to see if there was a Hurco emulator? I did find this site for a GCode reference? Not sure how old it is?
http://www.stonemachinery.com/support/document-library/g-code-list-hurco-ultimax-max.html

I'll see if my dolphinCAM had this type in it's driver base? But Jim's usually on the dime here. Will check for Hurco tomorrow when I'm in the office.

Good luck!


ecdez said:
I've been chasing gremlins on this machine for two weeks and finally got to cut some metal today only to find a new gremlin.


I have some code to cut a circle 1.339" in diameter (inside cut). Here's the code.

%
N10 G70 G17
N20 G40 G90
N30 S1000
N40 T1 M06
N50 G00 Z0.5
N60 S1000 M03
N70 X1.8954 Y0.4149
N80 Z0.0197
N90 G01 Z-0.06 F4

(All is good until here)

N100 G02 X1.3992 Y1.4519 I-0.2226 J0.5307 F12.0
N110 X1.6702 Y1.5211 I0.2736 J-0.5064
N120 X1.8954 Y0.4149 I0.0026 J-0.5755

(Back to good again)

N130 G00 Z0.5
N140 M05
N150 M02
E




I have two problems with it and both are equally disturbing.

#1 - circle comes out to just over 3.75" in diameter.

#2 - circle has a small (1/2" x 1/2") pac-man mouth in the 2 o-clock position


Machine is a Hurco with Ultimax. Code comes up on the display after being dripped in and it's the same as shown above. Double checked that everything is in inches. Generated the code twice with the same results.



Anyone have any ideas?
Click to expand...
 
Re: Code issue, please help. This stopped being fun a few days ago.

Thanks for the responses guys!

Little more info could have helped I suppose. I'm using sheet cam on the advice of someone on another forum because it's really simple and does 2.5d without all the bells and whistles and it has a Hurco post. I actually like CamBam alot but shyed away because I have to write my own post for that. I really just want to make parts.

In sheet cam the part shows up exactly like it should and even runs through the simulator correctly. Maybe the problem is in the post?




JimDawson said:
Check to see if the circle center is in absolute or incremental mode, it looks like it's incremental. Are you using a CAM program or are you generating this code on the machine.

EDIT:

I loaded your G-code in to my cam program, and yup, it has a PacMan mouth looking feature. Check your drawing to make sure there are no hidden lines or artifacts hiding. If you will post the hole center location from 0,0 and tool size, I'll run it through my CAM program and correct your G-code.
Click to expand...


I appreciate the offer but I have about 20 files I need to generate so I need to figure this out on what I have so I can crank some stuff out.


countryguy said:
I am still new, but was checking to see if there was a Hurco emulator? I did find this site for a GCode reference? Not sure how old it is?
http://www.stonemachinery.com/support/document-library/g-code-list-hurco-ultimax-max.html

I'll see if my dolphinCAM had this type in it's driver base? But Jim's usually on the dime here. Will check for Hurco tomorrow when I'm in the office.

Good luck!
Click to expand...

Thanks for the link. I have the original manual for the machine but I'll compare the info in the link to make sure it all lines up. The code portion of the manual was supplemental so I have no idea if it was original to the machine.


Marco Bernardini said:
The radius of the arc in N100 is 1.863, thus the diameter is 3.726.
Try here: http://www.calculatorsoup.com/calculators/geometry-plane/distance-two-points.php inserting your X,Y as (X1,Y1) and your I,J as (X2,Y2).
Click to expand...

Thanks for that link too, I was looking for something like that.


I'll try a different post in sheet cam and see what happens. I have a small machine that's running mach3 so I can possibly narrow the problem down to the post processor.


I downloaded the trial of BobCad and of course they contacted me to get me to buy the program. Unfortunately the trial version does not allow certain processes so I can't even see if their Hurco post will work correctly either. I have an email where their representative "guarantees" me it will work but once you spend the money what incentive do they have to make good on an email guarantee? Their site also has instructions on how to adjust you post should you need to but if I'm going to adjust a post why not just stick with CamBam and figure it out.

It's all really kind of frustrating but I am one step closer and happy to hear the problem is in the code and not some issue with the machine.
 
Re: Code issue, please help. This stopped being fun a few days ago.

ecdez said:
Thanks for the responses guys!

Little more info could have helped I suppose. I'm using sheet cam on the advice of someone on another forum because it's really simple and does 2.5d without all the bells and whistles and it has a Hurco post. I actually like CamBam alot but shyed away because I have to write my own post for that. I really just want to make parts.

In sheet cam the part shows up exactly like it should and even runs through the simulator correctly. Maybe the problem is in the post?
Click to expand...

I think you are correct, I suggest the problem is in the sheet cam post. I opened the g-code in CamBam and it is not a circle, and has a major dia of about 3.375.

Modifying a post processor is pretty easy in CamBam. The Hurco post looks a lot like Fanuc.
 
Re: Code issue, please help. This stopped being fun a few days ago.

I'm writing (just now!) a small "G-code to display" online converter based on this: https://github.com/fros1y/GView
The original creates a bunch of standalone files, while I'm trying to make a single online almost fancy image (yes, I'm lazy… as every hacker :biggrin:).
I think it's useful to test a few lines of G-code to see if the geometry is correct, before to deal with other more arcane codes.
If it works I'll donate it to the forum…
 
Re: Code issue, please help. This stopped being fun a few days ago.

Arc center vectors I and J are almost always measured as incremental distances from the start point of each arc to its center, so line 70 is the start point of the first arc. The X,Y coordinates in line 100 are the end point of the first arc and the start point for the second arc in line 110. Likewise, line 110 is the end of the second arc and the start of the third arc. Line 120 completes the circle.
I drew this out in AutoCAD with incremental center distances and it does trace a circle 1.1515" in diameter. Assuming the use of a 3/16" end mill, it would cut a 1.339" circle. The OP didn't mention cutter diameter or G42 offset.

If the control system requires absolute coordinates, they would be somewhere around I1.6728, J0.9457.

I am curious as to why the circle was divided into three arcs. I know that some older controls don't allow circular interpolation in more than one quadrant per block, so if that were the case there should be at least four blocks of code to cut each quadrant of a full circle. In the case of this program, there are only three blocks with arc angles of approximately 174
, 28 and 158 degrees.

Another option, if the control system allows, would be to program a full circle something like this:

N10 G70 G17
N20 G40 G90
N30 S1000
N40 T1 M06
N50 G00 Z0.5
N60 S1000 M03
N70 X1.8954 Y0.4149 (START POINT)
N80 Z0.0197
N90 G01 Z-0.06 F4
N100 G02 X1.8954 Y0.4149 I-0.2226 J0.5307 F12.0 (FULL CIRCLE with incremental I and J arc center coordinates)
N130 G00 Z0.5
N140 M05
N150 M02
E

A proper program to cut an internal circle should start near the center of the circle and move radially outward and arc into and out of the the circular path. This makes a smoother blend at the start and end points of the cut.


I forgot to mention that I am only familiar with HAAS and LinuxCNC controls so I don't know anything about Hurco.

 
Last edited:
Re: Code issue, please help. This stopped being fun a few days ago.

JimDawson said:
Modifying a post processor is pretty easy in CamBam. The Hurco post looks a lot like Fanuc.
Click to expand...

It looked pretty easy, I just didn't want to have to do it. Since I really like CamBam it may be worth the effort. I've heard the Hurco is pretty similar to Fanuc.





sinebar said:
I am curious as to why the circle was divided into three arcs. I know that some older controls don't allow circular interpolation in more than one quadrant per block, so if that were the case there should be at least four blocks of code to cut each quadrant of a full circle. In the case of this program, there are only three blocks with arc angles of approximately 178, 28 and 158 degrees.

Another option, if the control system allows, would to program a full circle something like this:

N10 G70 G17
N20 G40 G90
N30 S1000
N40 T1 M06
N50 G00 Z0.5
N60 S1000 M03
N70 X1.8954 Y0.4149 (START POINT)
N80 Z0.0197
N90 G01 Z-0.06 F4
N100 G02 X1.8954 Y0.4149 I-0.2226 J0.5307 F12.0 (FULL CIRCLE with incremental I and J arc center coordinates)
N130 G00 Z0.5
N140 M05
N150 M02
E

A proper program to cut an internal circle should start near the center of the circle and move radially outward and arc into and out of the the circular path. This makes a smoother blend at the start and end points of the cut.


I forgot to mention that I am only familiar with HAAS and LinuxCNC controls so I don't know anything about Hurco.
Click to expand...


Not sure why the three arcs either both both CamBam and SheetCam do it and have done it for both the Hurco and Mach3. Never had a problem with this on the small machine but Mach3 was a supplied post in CamBam. I'm just trying to sort out the Hurco. According to the manual Hurco can be programmed from the controller for a full circle and I think it had some code displayed with it so I believe it should be possible with one line of code it's just that I'd rather use a Cam program and drip than program the part into Ultimax.

There is an Option on CamBam to blend the start and end with a lead in and out but this section of the code is for the rough cut so that is not displayed. I do use it on the finish pass.

- - - Updated - - -

Sorry, forgot to mention I was using a .25" cutter but the program was wrote for a .1875" cutter. It wasn't until I ran the test that I realized I didn't have a 3/16" holder so I figured for a test I could wing it with the 1/4".
 
Re: Code issue, please help. This stopped being fun a few days ago.

I had to spend some time working on a BobCAD post for a router we have a while back and remember seeing something in there that affected how it output circles and arcs - I don't recall exactly what it was or how it worked, since that wasn't an area I was having trouble with, but just remember seeing it. Point being, there may be a setting in other software that is causing it to output arc segments rather than a full circle.
 
You must log in or register to reply here.
Back
Top