Problem 1.
The code below - genrated by hole pocketing - causes my Z axis servo to die by following error on line N190. I'm using the lates VM6 Std. On several occasions the latest Mach3 version xx.038 I'm using reproted of an error on in the R I J values but the simulation went OK though:
....
N90 (BEGIN - First Tool Macro)
N100 M901
N110 M6 T2
N120 M904
N130 G00 X175.2191 Y54.7403
N140 G00 Z5.0000
N150 M03 S16000
N160 (END - First Tool Macro)
N170 G01 Z-0.3650 F1000.0
N180 G17
N190 G03X175.2602Y55.0000Z-7.0000I-0.8691J0.2597 F2600.0
N200 G01 X175.2077 Y55.3023
N210 G03X175.2602Y55.0000Z-13.0000I-0.8577J-0.3023
.....
If I change the z movement to the previous line it works, like this:
...
N180 G17 Z-7
N190 G03 X175.2602 Y55.0000 I-0.8691 J0.2597 F2600.0
...
According to the post generator circle format there should be no z movement (EDIT: on line N190) when the circle is on XY plane (G17)? The plunge feed is set to F1000 which I suppose the Z movements should be using instead of the F2600 on the line N190?
The problem could also be caused by Mach, I'm just trying to figure the source of the problem.
Arc problems
Arc problems
Last edited by ftec on Mon Mar 01, 2010 4:36 am, edited 1 time in total.
Problem 2.
When pocketing a 129mm dia hole (2.5 axis pocketing) I can't get get it use spiral motion, it always generates linear segments. This causes a not so nice looking finish.
Problem 3.
Machining a fillet - edge of a large hole - using Horizontal Finishing also uses linear segments, haven't been able to change this to spiral patterns. The outcome on the work piece is not acceptable.
In Machining Preferences Arc output check boxes are not checked according to which I suppose arcs should be used instead of linear movements?
When pocketing a 129mm dia hole (2.5 axis pocketing) I can't get get it use spiral motion, it always generates linear segments. This causes a not so nice looking finish.
Problem 3.
Machining a fillet - edge of a large hole - using Horizontal Finishing also uses linear segments, haven't been able to change this to spiral patterns. The outcome on the work piece is not acceptable.
In Machining Preferences Arc output check boxes are not checked according to which I suppose arcs should be used instead of linear movements?
I haad to retype this entire reply since the forum (as it does sometimes) returned the "automatic insertion" error. I really wish this would get fixed, as I don't always remember to save the reply to notepad "just in case".
Sounds like your power supply is not powerful enough for 3 axis moves. If Mach3 is not erroring out on the code, it is not a CNC code issue. Following error is a machine dynamics issue. Try running the line of code with a significantly reduced feedrate to make more current available to the z axis servo.
To ouput toolpaths with arc rather than lines, enable cut arc filtering on the advanced tab of the MOP with a tolerance of say .002 and change the cut tol on the cut parameters tab to .001, then regenerate.
In my experience the helical entry moves always generate and post as linear moves. My 1995 VMC hates that kind of code (shudders) so I always use the linear entrance method, with an angle of 7 degrees and a length as long as will fit.
Joe
Sounds like your power supply is not powerful enough for 3 axis moves. If Mach3 is not erroring out on the code, it is not a CNC code issue. Following error is a machine dynamics issue. Try running the line of code with a significantly reduced feedrate to make more current available to the z axis servo.
To ouput toolpaths with arc rather than lines, enable cut arc filtering on the advanced tab of the MOP with a tolerance of say .002 and change the cut tol on the cut parameters tab to .001, then regenerate.
In my experience the helical entry moves always generate and post as linear moves. My 1995 VMC hates that kind of code (shudders) so I always use the linear entrance method, with an angle of 7 degrees and a length as long as will fit.
Joe
-
Mitch Heynick
- Posts: 488
- Joined: Wed Aug 01, 2007 4:15 pm
- Location: Switzerland
- Contact:
I can't help you with the main issues you posted about - but as far as the "automatic insertion" problem... I experienced this many times until I learned the trick...I haad to retype this entire reply since the forum (as it does sometimes) returned the "automatic insertion" error. I really wish this would get fixed, as I don't always remember to save the reply to notepad "just in case".
This happens when it takes you awhile to finish your post, more than about 3 or 4 minutes and you will get this message - it's like your privileges have expired or something... So, as soon as I have a long reply or have waited a while before hitting the Submit button, I hit PREVIEW first... You will then see your post previewed and it resets your counter. If you then hit Submit after the preview appears, it will go in no problem. Never had a problem after that... --Mitch
-
MecSoft Support
- Posts: 2405
- Joined: Wed Aug 01, 2007 4:15 pm
- Location: Irvine, CA, USA
- Contact:
Re: Problem1
N190 G03X175.2602Y55.0000Z-7.0000I-0.8691J0.2597 F2600.0
Line N190 is performing a helical move. The macro's for helical interpolation is defined under the Helix/Spiral tab in the post processor.
Make sure your machine can handle helical interpolation. If the machine does not support helical interpolation, you can output Helix motions as linear segments. This can be changed under Machining Preferences.
Re: Problem2
Use offset cuts instead of spiral cuts from the pocketing cut parameters tab. The offset cut pattern would traverse in successive uniform offsets of the selected curve.
Make sure you have output arcs as linear segments unchecked under Machining Preferences.
Re Problem3
Arcs can be fit to 3 axis toolpath in XY XZ and YZ planes using the Toolpath Editor. This feature is available in Pro configuration.
N190 G03X175.2602Y55.0000Z-7.0000I-0.8691J0.2597 F2600.0
Line N190 is performing a helical move. The macro's for helical interpolation is defined under the Helix/Spiral tab in the post processor.
Make sure your machine can handle helical interpolation. If the machine does not support helical interpolation, you can output Helix motions as linear segments. This can be changed under Machining Preferences.
Re: Problem2
Use offset cuts instead of spiral cuts from the pocketing cut parameters tab. The offset cut pattern would traverse in successive uniform offsets of the selected curve.
Make sure you have output arcs as linear segments unchecked under Machining Preferences.
Re Problem3
Arcs can be fit to 3 axis toolpath in XY XZ and YZ planes using the Toolpath Editor. This feature is available in Pro configuration.
OK, I need to study this closer, not sure if Mach can handle this. EDIT: I just learned that there may be an issue with Mach's 3 axes circular interpolation and G61 exact stop was suggested to be used. I'll also check the dZ and the feedrate, maybe these will help.MecSoft Support wrote: Re: Problem1
N190 G03X175.2602Y55.0000Z-7.0000I-0.8691J0.2597 F2600.0
Line N190 is performing a helical move. The macro's for helical interpolation is defined under the Helix/Spiral tab in the post processor.
Make sure your machine can handle helical interpolation. If the machine does not support helical interpolation, you can output Helix motions as linear segments. This can be changed under Machining Preferences.
There must be something I'm doing wrong as I've tried offset cut too, everything I do results linear segments. All check boxes are unchecked in Machining Preferences.Re: Problem2
Use offset cuts instead of spiral cuts from the pocketing cut parameters tab. The offset cut pattern would traverse in successive uniform offsets of the selected curve. Make sure you have output arcs as linear segments unchecked under Machining Preferences.
I see. Then how would you suggest I program the large fillet in the pic attached?Re Problem3
Arcs can be fit to 3 axis toolpath in XY XZ and YZ planes using the Toolpath Editor. This feature is available in Pro configuration.
- Attachments
-
- chamfer.JPG (41.2 KiB) Viewed 18105 times
Last edited by ftec on Mon Mar 01, 2010 4:30 pm, edited 1 time in total.
PS. Then how should I set things up for Hole Pocketing to make the plunge into the work piece, then run a circle move, then offset a tad inwards (or outwards) then make the next circle etc... each using the G2 or G3 command?
Btw. the help file for hole pocketing is probably out of date for the Entry/exit as the 'Create full 360 helixes only' and 'output each helix individually' are missing from the help.
Btw. the help file for hole pocketing is probably out of date for the Entry/exit as the 'Create full 360 helixes only' and 'output each helix individually' are missing from the help.
Following error is reported when actual movement deviation from commanded movement exceeds the programmed threshold.Fennotek wrote:Nope, there is plenty of power, it is not a machine issue. Mach reports an error when machining but not when simulating.scudzuki wrote:
Sounds like your power supply is not powerful enough for 3 axis moves. ...
Joe
Whatever is reporting this error is stretching the truth.
If the error is with Mach itself, it must believe it is commanding movement in Z when it is not, due to the bug you alluded to. There is no change in Z so Mach reports following error, which is erroneous since Mach is open loop (unless you get one of Bob Campbell's feedback boards and use it in conjunction with his BOB). Since it doesn't expect to see commanded axis movement in simulation mode it produces no following error.
I spent several thousand dollars to upgrade to a version with the toolpath editor when I was getting lines instead of arcs.
I later learned that I got the same results, without editing the toolpath, using arc fitting when generating the MOP. Coulda saved a bundle of money if I'd known.
I assumed you were using the spiral strategy for pocketing.
Joe
-
MecSoft Support
- Posts: 2405
- Joined: Wed Aug 01, 2007 4:15 pm
- Location: Irvine, CA, USA
- Contact:
The error reporting I meant was the R I J error when machining but not when simulating - as I said in my original post. Probably something extremely rapid - something exceeding the allowed Z acceleration defined for Z in Mach and not seen by the Mach simulation - is happening on N190 because a fuse would break if the motor Peak Current had been exceeded (and they don't have the time to do that). Total current for all motors is not exceeded either.scudzuki wrote:Following error is reported when actual movement deviation from commanded movement exceeds the programmed threshold.Fennotek wrote:Nope, there is plenty of power, it is not a machine issue. Mach reports an error when machining but not when simulating.scudzuki wrote:
Sounds like your power supply is not powerful enough for 3 axis moves. ...
Joe
Whatever is reporting this error is stretching the truth.
...
Joe
PS: The material is soft plastic. The Z motor is quite capable to make the 3.175 mm tool to penetrate deep into the material as I learned when the spindle did not start (previous Mach version I used).
This is my hobby and therefore I'm still in the beginning of the learning curve for VM but all the mistakes I make are very good teachers.
-
MecSoft Support
- Posts: 2405
- Joined: Wed Aug 01, 2007 4:15 pm
- Location: Irvine, CA, USA
- Contact:
Glad to be there!MecSoft Support wrote:Glad to have you as a Pro customer!
You probably are aware of the way how my Pro licence upgrade was arranged. This is a chance other individuals and small companies like mine would probably like to be aware of. At least it brought you one new Pro customer.
Regards,
Risto A.
It seems that the reson for this was that 'Create Single Flat Area Regions' created the large circle in the 3D model as polyLINE and not as a circle. Once I drew a circle for bounding region it worked.Fennotek wrote:Problem 2.
When pocketing a 129mm dia hole (2.5 axis pocketing) I can't get get it use spiral motion, it always generates linear segments. This causes a not so nice looking finish.