PDA

View Full Version : Problem Guys I am having a problem with RhinoCam and Mach 3 G02/G03



FoxCNC1
04-25-2015, 10:43 PM
I am trying to cut a CBORE as shown below with the following code.
The rhinocam simulation shows it cut correctly, however when the code is loaded into Mach3, I don't see the same tool path and the cut is incorrect. The only way around this was to change the arc output setting in Rhinocam and output as lines. However if I am not mistaken, Mach 3 does interpret G2 and G3 codes doesn't it?


G00 G49 G40.1 G17 G80 G50 G90
G20
(Hole Pocketing_CBORE 0.3)
M6 T3
M03 S13500
G00 Z1.5000
X-5.1574 Y0.6252
G01 Z0.0250 F60.0
G17
G02X-5.1573Y0.6250Z-0.1500I-0.0952J-0.0002 F190.0
X-5.4578I-0.2051J0.0000
X-5.0475I0.2052J0.0000
G01 X-5.1573
X-5.1574 Y0.6252
G02X-5.1573Y0.6250Z-0.3000I-0.0952J-0.0002
X-5.4578I-0.2051J0.0000
X-5.0475I0.2052J0.0000
G01 X-5.2526
G00 Z1.5000
M5 M9
M30


http://i10.photobucket.com/albums/a146/Profoxcg/rhinoG02_zpshjvdmkb1.jpg (http://s10.photobucket.com/user/Profoxcg/media/rhinoG02_zpshjvdmkb1.jpg.html)

Mach 3.

The cut piece resembles the Mach 3 path.

http://i10.photobucket.com/albums/a146/Profoxcg/G02_zpsupyfq00g.jpg (http://s10.photobucket.com/user/Profoxcg/media/G02_zpsupyfq00g.jpg.html)

jalessi
04-25-2015, 11:46 PM
FoxCNC1,

I am guessing however have you tried switching the IJ Mode setting?

Jeff...

FoxCNC1
04-25-2015, 11:58 PM
was not aware of that setting, but when I made the change the path looks extremely large - out of scale.

jalessi
04-26-2015, 12:06 AM
Disregard the suggestion if it did not help.

ger21
04-26-2015, 07:56 AM
RhinoCAM is not outputting all the code. What you see in Mach3 is all that RhinoCAM is sending.

Never used RhinoCAM, so can't help any more than that.

FoxCNC1
04-26-2015, 09:00 AM
Let me check / compare code before and after output. Its very weird.
to rule out that I am not crazy, Mach 3 can interpret arcs and helix?

ger21
04-26-2015, 09:10 AM
Yes

FoxCNC1
04-26-2015, 09:43 AM
Is there a particular way Mach3 likes the code for arcs and helix?

Here is the post editing options, maybe I am missing something:
I appreciate the help.

http://i10.photobucket.com/albums/a146/Profoxcg/Helix_zpsdmrnpb02.jpg (http://s10.photobucket.com/user/Profoxcg/media/Helix_zpsdmrnpb02.jpg.html)

http://i10.photobucket.com/albums/a146/Profoxcg/circle_zps4ecfsgvy.jpg (http://s10.photobucket.com/user/Profoxcg/media/circle_zps4ecfsgvy.jpg.html)

ger21
04-26-2015, 09:51 AM
I believe that the Arc Center should be "Vector from Start to Center".

FoxCNC1
04-26-2015, 09:38 PM
nothing works. very weird.
The only way to get that cut correctly is to output helix and spirals as lines. I have a PMDX-126 breakout. Would that have anything to do with it?

ger21
04-27-2015, 11:50 AM
RhinoCAM is not outputting the g-code. It's 100% a RhinoCAM issue. It's not that mach3 is not running the code correctly. The code is NOT there.

FoxCNC1
04-27-2015, 11:56 AM
RhinoCAM is not outputting the g-code. It's 100% a RhinoCAM issue. It's not that mach3 is not running the code correctly. The code is NOT there.

Thanks I will contact customer service then. Maybe they can help with what is going on with my post.

beezerlm
04-28-2015, 10:54 AM
Hi FoxCNC1. Are you sure that you selected all MOPS for posting? It looks like a lot of code is missing?

FoxCNC1
04-28-2015, 11:10 AM
Hi FoxCNC1. Are you sure that you selected all MOPS for posting? It looks like a lot of code is missing?

Yep, doesn't make a different if I select the MOP or the SETUP. I even made a different file just rule out corruption and nothing.
I am on 2014 from 2012..I don't like how 14 does the "tabs" to hold down parts either..

beezerlm
04-28-2015, 11:43 AM
Could you upload or send me the 3dm file so I can post it on my end and see if I get the same result?

FoxCNC1
04-28-2015, 12:02 PM
yeah I would appreciate that.
I got a reponse from support, and they are saying that maybe my CNC Controller does not support spiral interpolation. What is the "controller" I thought that was Mach 3? or it is the UC100 USB interface or the PMDX-126 driving my system.. can you please clarify this?

PM me your e-mail.

beezerlm
04-28-2015, 12:35 PM
I believe they are talking about mach 3. I have thread-milled with mach 3 in the past. It should be able to handle that. PM sent.

ger21
04-28-2015, 07:50 PM
I got a response from support, and they are saying that maybe my CNC Controller does not support spiral interpolation.

The spiral moves are not in your g-code.

Mach3 is the control, but it can't read what's not there.

FoxCNC1
04-28-2015, 07:55 PM
thank you for the clarification Ger. Make sense, I was told in the e-mail it is not set up.

beezerlm
04-29-2015, 02:24 PM
Well I tried getting Mach3 to perform a true spiral and I can't seem to find any Rhino output that will work with Mach3. There is a "circular pocket" wizard in Mach3 that will create the spiral code for you using a series of 180 degree arcs, but that does not solve your problem with Rhino. I don't think Mach3 will support a full spiral without breaking it up into arc events. Here are screen shots of the wizard and toolpath:

278406

278408

FoxCNC1
04-29-2015, 02:41 PM
thanks, I guess we all learned something need.

ger21
04-29-2015, 06:35 PM
Well I tried getting Mach3 to perform a true spiral

A "true" spiral can not be made with G2/G3 arcs, as a true spiral has a constantly changing radius.

FoxCNC1
04-29-2015, 06:49 PM
Ger, can you get spirals out of whatever cam software you use?

ger21
04-29-2015, 08:16 PM
Yes.

My guess is that you're missing something in RhinoCAM.

RhinoCAM is showing the toolpaths on the screen, but it's not outputting the g-code for them, for whatever reason.

beezerlm
04-29-2015, 10:56 PM
Some machines use a G2.1 or G3.1 to perform "True" spiral milling by use of an added variable to control the "pitch" of the spiral. It looks to me like this is what Rhinocam is set up for.

Correct me if I am wrong, but it does not look like Mach3 will accept this kind of command.

yham
06-21-2016, 12:33 PM
A bit old post, but I stumbled with the same problem. Fox, have you found a solution?

It is interesting, when I have a spiral machining, everything is ok, G code is generated and no problem with mach. If I use round pocket strategy, there is a problem - spiral is not g coded. I assume, mach post has an issue. Didn't compare mach posts from rhinocam and mach web.

FoxCNC1
06-21-2016, 03:40 PM
Hi there, not that I recall.

awerby
06-21-2016, 04:14 PM
I don't think there's a problem with Rhinocam producing helical toolpaths; the question of whether they are "true" or not is more philosophical than practical. If Mach3 can't deal with G02/G03 spirals, it will output them as a series of short segments, which, if they're short enough, can't be distinguished from "true" spirals.

yham
06-21-2016, 05:32 PM
I really think it is a problem with Rhinocam. Spiral machining makes spiral toolpath and Rhinocam generates code that doesn't have g2 or g3 and spirals are made of segments, and as such, they run through mach without errors. Problem rise up with hole pocketing, Rhinocam's post for mach generates g2 and g3 when spiral should start. (I don't think it makes sense, but maybe I am wrong) and this is the place where mach reports error. It is strange that cam will not make segmented path with hole pocketing, as it does with spiral machining. To me those toolpaths looks the same.

Here is where error is in hole pocketing:

G00 G49 G40.1 G17 G80 G50 G90
G20
.
.
.
.
X0.1250 Y0.0000 Z-0.2500 - end of lead in helix
G17
G03X-1.8743I1.8743J0.0000
X1.8743I-1.8743J0.0000
G01 X0.0000
G00 Z0.2500
M5 M9
M30

There should be a lot of code, because spiral is not short, but somehow, there is nothing of it.

Have no idea is there a problem with mach, it can not interpret spiral (helix is ok) or there is a problem with mach post in rhinocam.

thanks

p.s figured out that basically, a spiral code is missing. Why it is not generated, I don't know, when it may be generated as a segmented spiral.

awerby
06-22-2016, 05:23 PM
It could be that there's something wrong with your I J K settings that's triggering the error messages. The Mach3 manual talks about how they work: CNC Mach3 G-Codes (http://machmotion.com/cnc-info/g-code.html) . Here's a thread on this site that talks about them: http://www.cnczone.com/forums/mach-software-artsoft-software-/95246-mach3-arc-problems.html

If RhinoCAM isn't telling it to do it the way you want it to, you might have to edit the Mach3 post so it puts in the right G code, either G90.1 for absolute, or G91.1 for incremental.