wells index m40 backwards z

Discussion of post processors for various CNC machines

wells index m40 backwards z

Postby swatson144 » Mon Apr 20, 2015 7:34 pm

when I finish the cam cycle and load the program into the mill the z axis is seeming to move toward backwards ie plunging in the positive direction . Both the Bridgeport and wells index need to move negative to cut. I assume this to be an easy fix in the post?

I have tried Centroid since the WI is a centroid controller. and a couple other POSTs.

I read for a while but didn't find an answer. I seem to be overlooking something in the .con

Steve
swatson144
 
Posts: 9
Joined: Sat Dec 27, 2014 11:32 pm

Re: wells index m40 backwards z

Postby Randy » Tue Apr 21, 2015 12:10 am

Hi Steve, and welcome to the forum. There is nothing that can be set up in MeshCAM--it (as well as other CAM programs) output gcode in a right-handed coordinate system, defined as tool motion relative to the workpiece.

P1070830.png
CNC gang-sign
P1070830.png (387.5 KiB) Viewed 1822 times

Make sure you have the axes set up in your control program (which is where you need to make the settings). If you're using the quill for Z it moves downwards for Z- moves (you are moving the tool), but if you're using the knee for Z it moves up for Z- moves (you are moving the workpiece). If you need to reverse an axis movement make sure you also reverse the sense of the jogging so it works the correct direction.

Randy
All opinions in this post are mine alone. I am not a MeshCAM employee, I do not have a financial interest in MeshCAM, nor do I speak for MeshCAM. MeshCAM user since Beta 5 in 2003. viewtopic.php?f=11&t=15333 :ugeek:
Randy
 
Posts: 1812
Joined: Wed May 14, 2008 9:50 am
Location: North Texas, USA

Re: wells index m40 backwards z

Postby swatson144 » Tue Apr 21, 2015 12:24 pm

Thank you for the fast response Randy. Both mills are configured for Rhand coordinate system. It is good to know that is not the problem. It seems that for some reason the code is coming out as if it was for Z being the knee not the spindle. I am using the spindle for Z with - being moving the tool into the work and Z+ moving for clearance.

Just as a note. It is a strange setup at work internet is available only on computers that will not accept any media, so it is difficult for me to paste/attach code or the .jpg as a reference. The CNC attached network is fair game for mem sticks etc. but no internet. That is the reason for no examples. If I don't work my way through today I'll include examples tonight from home.

I bought Meshcam in late Dec. of last year and am just now starting to work with it. Most likely I jumped in above my head with the current project and probably should draw a simple design and get that running then go on to .jpg and engraving. It's a direction I'd like to go with the mills for work that is too heavy for the engravers. Maybe I should upgrade to Pro/Art?

Currently I have been using BobCad and Millwrite for valve handwheels etc. so I'm not a complete newby, and I think MeshCAM will be a great addition to the line up.

I'll work to get something done today
Steve
swatson144
 
Posts: 9
Joined: Sat Dec 27, 2014 11:32 pm

Re: wells index m40 backwards z

Postby Randy » Tue Apr 21, 2015 4:12 pm

It seems that for some reason the code is coming out as if it was for Z being the knee not the spindle.

The Gcode wouldn't know that, Steve. Gcode is just movements in space and is independent of machine. You can examine the MeshCam gcode output in a text editor. If you have zeroed Z at the top of your stock, the retract height will be positive Z value and all cutting will be negative Z values. You only need to go 10 or so lines in to find the first plunge into the material. If you have zeroed Z at the bottom of the stock, all Z's will be positive but cutting Z values will be less than the retract Z value.

You can verify the axes motion with a simple hand-written program also. Zero the axes well up above the table (a couple inches) and run

Code: Select all
G20 G90
G1 X1.0000 F10
G1 Z-1.0000
G1 X0.0000
G1 Z0.0000

This moves (as seen from the table) the cutter 1 inch to the right, 1 inch down, 1 inch to the left and 1 inch up to the starting point. The first line sets up inch and absolute moves.

vertsquare.png
vertsquare.png (2.12 KiB) Viewed 1808 times

There is nothing special in the Cenroid post
Code: Select all
; MeshCAM config
; This config is the Mach2 machine controller
; 12/10/2012 - Copied config from Mach3
;
DESCRIPTION = "Centroid-Inch(*.cnc)"
FILE_EXTENSION = "cnc"
UNITS=INCH
;Feeds
FORMAT = [F|#|F|1.1]
;Moves
FORMAT = [I|@|I|1.4]
FORMAT = [J|@|J|1.4]
FORMAT = [X|#|X|1.4]
FORMAT = [Y|#|Y|1.4]
FORMAT = [Z|#|Z|1.4]
;
;
COMMENT_START = "("
COMMENT_END = ")"
;
START = "%"
START = "(FILENAME: [FILENAME])"
;;the following sets the stock for CutViewer
START = "([CUTVIEWERSTOCK])"
START = "G20G64G17"
START = "G90"
;
TOOLCHANGE = "([CUTVIEWERTOOL])"
TOOLCHANGE = "M6 [T]"
TOOLCHANGE = "M3 [S]"
;
RAPID_RATE_MOVE        = "G0[X][Y][Z]"
;
FIRST_FEED_RATE_MOVE   = "G1[X][Y][Z][F]"
FEED_RATE_MOVE         = "[X][Y][Z]"
;
FIRST_CW_ARC_MOVE = "G2[X][Y][I][J][F]"
CW_ARC_MOVE = "G2[X][Y][I][J]"
;
FIRST_CCW_ARC_MOVE = "G3[X][Y][I][J][F]"
CCW_ARC_MOVE = "G3[X][Y][I][J]"
;
;
END = "M5"
END = "M30"

and as I said before, the post doesn't set the move coordinates, it just formats the output for a specific machine. This is set up for absolute inch coordinates and standard X-Y plane for the arcs. You can see that the X Y Z coordinates are just written out and there is no provision for changing their sign (which would actually be a dangerous thing to do... :shock: )

Randy
All opinions in this post are mine alone. I am not a MeshCAM employee, I do not have a financial interest in MeshCAM, nor do I speak for MeshCAM. MeshCAM user since Beta 5 in 2003. viewtopic.php?f=11&t=15333 :ugeek:
Randy
 
Posts: 1812
Joined: Wed May 14, 2008 9:50 am
Location: North Texas, USA

Re: wells index m40 backwards z

Postby swatson144 » Tue Apr 21, 2015 9:04 pm

Thanks again Randy. It turned out much as I had guessed... The code was so intense that I was mistaken on what it was doing /when. IE it WAS (correctly) going + to move but because it was such a short move there was no rapid involved and I didn't see it as a clearance move. It was 60k lines and I never really got past aux Graph

I got a successful run of my logo this afternoon. I imported it to ACAD and saved as a .dxf which removed a lot of detail for the test. then saved it as a .bmp and put it into MeshCAM to work with. I know that was a lot of un needed steps but it quickly reduced the program to a reasonable size (5K lines) coming from a picture.

I'm happy. I got results and more confidence in MeshCAM. Now It's just tweaking and trying different projects.

Thanks for the help and the great software.

Steve
swatson144
 
Posts: 9
Joined: Sat Dec 27, 2014 11:32 pm

Re: wells index m40 backwards z

Postby Randy » Tue Apr 21, 2015 9:30 pm

Steve, you're welcome for the help (but it sounds like you knew your stuff anyway :) ) and you can thank Robert for the software. MeshCAM is a one-man effort and Robert is The Man.

Randy
All opinions in this post are mine alone. I am not a MeshCAM employee, I do not have a financial interest in MeshCAM, nor do I speak for MeshCAM. MeshCAM user since Beta 5 in 2003. viewtopic.php?f=11&t=15333 :ugeek:
Randy
 
Posts: 1812
Joined: Wed May 14, 2008 9:50 am
Location: North Texas, USA


Return to Post Processors

cron