Mach3 ignoring A coordinates when using YtoA PostProcessor?

Topics related to wrapped rotary machining in Aspire or VCarve Pro

Mach3 ignoring A coordinates when using YtoA PostProcessor?

Postby GF357 » Thu May 05, 2016 7:20 pm

I recently added a Sherline 4" rotary table to my CNCRP Pro 48X96, and after getting the motor configured and moving right, I'm noticing some odd behavior from even simple toolpaths created with VCarve Pro 8 and the Mach3 YtoA post processor...

A toolpath of a simple profile of a box only produces a line cut along the X axis. The first problem seems to occur at N260, the A- move. It appears that Mach just ignores it, as there's no delay on the X axis moves. Same for the A+ move in N280. I can manually move the A axis with the hotkeys and the pendant, and A axis commands prior to line 260 will cause the the table to move into correct position.

Anyone have any ideas?


Code: Select all
( Box1YtoA )
( File created: Thursday May 05 2016 - 09:50 AM)
( for Mach2/3 from Vectric )
( Material Size)
( X= 4.000, Z= 0.688)
( Diameter = 1.3760 Inches)
( Y Values are wrapped around the X axis )
( Y Values are output as A )
()
(Toolpaths used in this file:)
(Box1)
(Tools used in this file: )
(1 = End Mill {0.250 inch})
N130 G00G20G17G90G40G49G80
N140 G70G91.1
N150 T1M06
N160 G00G43Z2.0000H1
N170 S12000M03
N180(Toolpath:- Box1)
N190()
N200 G94
N210 A0.0000 X0.0000 Z2.0000 F100.0
N220 G00 X-1.0000 A83.2787 Z0.9380
N230 G00 X-1.0000 A83.2787 Z0.6880
N240 G1 X-1.0000 A83.2787 Z0.5510 F30.0
N250 G1 X1.0000 A83.2787 Z0.5510 F100.0
N260 G1 X1.0000 A-83.2787 Z0.5510
N270 G1 X-1.0000 A-83.2787 Z0.5510
N280 G1 X-1.0000 A83.2787 Z0.5510
N290 G00 X-1.0000 A83.2787 Z0.9380
N300 G00 Z2.0000
N310 G00 A0.0000 X0.0000
N320 M09
N330 M30
%
GF357
 
Posts: 7
Joined: Tue Nov 17, 2015 4:54 pm
Model of CNC Machine: CNCRP PRO48X96

Re: Mach3 ignoring A coordinates when using YtoA PostProcess

Postby IslaWW » Thu May 05, 2016 9:42 pm

If you type in an A axis move from the keyboard, does the rotary axis move? Example: G0 A90 etc.
Gary Campbell
CNC Technology & Training
Control & ATC Retrofits
GCnC411 (at) gmail.com
User avatar
IslaWW
Vectric Wizard
 
Posts: 846
Joined: Wed Nov 21, 2007 11:42 pm
Location: Marquette, MI, USA
Model of CNC Machine: SideWinder ATC & CNC Mill on WinCNC

Re: Mach3 ignoring A coordinates when using YtoA PostProcess

Postby GF357 » Thu May 05, 2016 9:59 pm

Yes it does. The A axis also moves in the code I posted prior to line 260, as well. This is probably a Mach3 issue and not so much a Vectric post processor issue, but I figured I'd start here to see if anyone has dealt with this before. I noticed the output of the YtoA post processor (compared to normal Mach2/3) makes some seemingly cosmetic changes to the G code, most notably the spacing between coordinates and the locations of a few other things. I tried editing the code to remove the spacing or putting the G1 A# moves on their own line, and all of the changes had the same result as the original - no movement.
GF357
 
Posts: 7
Joined: Tue Nov 17, 2015 4:54 pm
Model of CNC Machine: CNCRP PRO48X96

Re: Mach3 ignoring A coordinates when using YtoA PostProcess

Postby Leo » Thu May 05, 2016 10:14 pm

On line 260 the A changes from positive to negative.

There may be a setting to allow Mach3 to recognize the "-" A
Imagine the Possibilities of a Creative mind

www.leosworkshop.com
User avatar
Leo
Vectric Wizard
 
Posts: 2417
Joined: Sat Jul 14, 2007 3:02 am
Location: East Freetown, Ma.
Model of CNC Machine: 1300 x 1300 x 254

Re: Mach3 ignoring A coordinates when using YtoA PostProcess

Postby GF357 » Thu May 05, 2016 10:27 pm

The change in the A value from positive to negative is to get the rotary table to move CCW. The toolpath being cut is symmetrical around the reference point. Typing G1 A# and G1-# commands in the MDI window make the A axis move as it should.
GF357
 
Posts: 7
Joined: Tue Nov 17, 2015 4:54 pm
Model of CNC Machine: CNCRP PRO48X96

Re: Mach3 ignoring A coordinates when using YtoA PostProcess

Postby rdean33422 » Thu May 05, 2016 11:42 pm

I don't know anything about Sherline products but I copied your code over to mach3 and ran a simulation. I works fine. I also single stepped through the program and the A axis worked as expected on every line.

Sorry no help here.

Ray
rdean33422
Vectric Craftsman
 
Posts: 109
Joined: Wed Mar 30, 2011 5:55 pm
Model of CNC Machine: RF31, 4X8 Router both CNC

Re: Mach3 ignoring A coordinates when using YtoA PostProcess

Postby GF357 » Fri May 06, 2016 12:36 am

The Sherline rotary table isn't the issue I don't think, as I've changed the motor to a CNCRP NEMA 23 stepper to match the rest of the table and it has been configured in Mach3... except for this problem. It moves using the hotkeys, pendant, and even with typing G00 and G1 commands in the MDI command line, just not throughout the toolpath. I've posted the same question over at the Mach3 forum, we'll see what they come up with.

http://sherline.com/product/3700-cnc-cn ... ary-table/
GF357
 
Posts: 7
Joined: Tue Nov 17, 2015 4:54 pm
Model of CNC Machine: CNCRP PRO48X96

Re: Mach3 ignoring A coordinates when using YtoA PostProcess

Postby TReischl » Sat May 07, 2016 1:22 am

Don't have my Mach manual right at the moment, but, something is telling me that you are missing a setting in Mach.

Something to do with how feedrates are set in Mach. . . seems to me I had a similar problem when I set mine up, but that was quite a while ago.
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 1966
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X8 RP 2010 Screenset

Re: Mach3 ignoring A coordinates when using YtoA PostProcess

Postby IslaWW » Sat May 07, 2016 3:43 pm

Any chance there is an A soft limit around Zero or just under that would stop negative commands?
Gary Campbell
CNC Technology & Training
Control & ATC Retrofits
GCnC411 (at) gmail.com
User avatar
IslaWW
Vectric Wizard
 
Posts: 846
Joined: Wed Nov 21, 2007 11:42 pm
Location: Marquette, MI, USA
Model of CNC Machine: SideWinder ATC & CNC Mill on WinCNC

Re: Mach3 ignoring A coordinates when using YtoA PostProcess

Postby GF357 » Sat May 07, 2016 4:45 pm

The problem was found... how Mach3 handled it was a little surprising and disappointing at the same. In the general config I had 360 Rollover enabled, and this would not allow negative A moves in a toolpath but would allow them to be issued via the MDI. So the same command in a toolpath would get no response while typed into the MDI it would work.

All seems to be working now, thanks for the help.
GF357
 
Posts: 7
Joined: Tue Nov 17, 2015 4:54 pm
Model of CNC Machine: CNCRP PRO48X96


Return to Wrapped Rotary Machining

Who is online

Users browsing this forum: No registered users and 2 guests