"W" AXIS POST PROCESSOR

This forum is for general discussion about Aspire
Post Reply
brockadeau
Vectric Craftsman
Posts: 131
Joined: Fri Mar 24, 2006 12:16 am
Location: Massachusetts
Contact:

"W" AXIS POST PROCESSOR

Post by brockadeau »

I have a cnc with two heads, a "z" axis and a "w' axis in addition to the x and y axis. I am trying to modify the WinCNC inch post processor to output the w in place of the z. I tried replacing all the "z's" with "w's" in the post processor but it doesn't load because it doesn't recognize the w value. Any ideas? thanks--Jack

Brad.At.CNC
Vectric Apprentice
Posts: 8
Joined: Thu Apr 13, 2017 6:51 pm
Model of CNC Machine: Thermwood 3 Axis
Location: St. Zotique, Quebec, Canada
Contact:

Re: "W" AXIS POST PROCESSOR

Post by Brad.At.CNC »

I am not sure about your particular CNC control system, but with the one that I have worked with, the axis for the second head is usually not referred to directly. Rather, a command is inserted that "redirects" the Z references that follow it to that second vertical axis. There is a related command that "breaks" the previous axis "redirect".

Similarly, if the two heads are to be used together or "tied", a command is inserted to direct the machine to have the second vertical axis "follow" (to be "tied" to) the first/primary one. There is a related command that "breaks" the previous axis "tie".

Perhaps a review of your machines' manual will document a similar feature/function/command.

eph210
Vectric Craftsman
Posts: 192
Joined: Mon Mar 11, 2013 1:23 am
Model of CNC Machine: Stinger 1 and Mabel, both with 4 axis
Location: southern Alberta, Canada

Re: "W" AXIS POST PROCESSOR

Post by eph210 »

Make sure your WinCNC.INI file acknowledges The W axis. It needs to be specified in the AXISCHAR list.
You also will need to set up the AXISSPEC for the W axis.
Save a backup copy of the .INI file before changing anything.
I have found emailing WinCNC to be very helpful in setting up my machine. They probably have a PP already for a dual head machine.

Euan

brockadeau
Vectric Craftsman
Posts: 131
Joined: Fri Mar 24, 2006 12:16 am
Location: Massachusetts
Contact:

Re: "W" AXIS POST PROCESSOR

Post by brockadeau »

I have WinCNC set up with the "W" axis and I am currently using it by manually editing the gcode file by changing the Z's to W's in a text editor. I am just hoping there is an easier and faster way.

User avatar
Adrian
Vectric Archimage
Posts: 10624
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: "W" AXIS POST PROCESSOR

Post by Adrian »

You need to change the prefix character in the variable definitions for the Z axis in your post processor. Best to create a new one and change the POST_NAME to reflect it as being a W axis one.

Where you have lines like these:

Code: Select all

VAR Z_POSITION = [Z|C|Z|1.4]
VAR Z_HOME_POSITION = [ZH|A|Z|1.4]
You need to change them to be:

Code: Select all

VAR Z_POSITION = [Z|C|W|1.4]
VAR Z_HOME_POSITION = [ZH|A|W|1.4]

User avatar
IslaWW
Vectric Wizard
Posts: 1303
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: The Ultimate Woodworking Machine
Location: Marquette, MI, USA

Re: "W" AXIS POST PROCESSOR

Post by IslaWW »

You will want to look at the L11, L12 and L13 commands. Most likely L12 WZ.

The code will allow you to swap the W and Z axis (with code designated as "Z") and return to normal operation. I would do the swap by either by making a postP with the command in the header, adding it into the "TOOL_NOTES" and toggling it on as needed, or simply be hand entering it before a file is run.

Dont forget the "Toggle Off" version of which ever you use.
L codes.JPG
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com

User avatar
IslaWW
Vectric Wizard
Posts: 1303
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: The Ultimate Woodworking Machine
Location: Marquette, MI, USA

Re: "W" AXIS POST PROCESSOR

Post by IslaWW »

I ran this by the guys at Microsystems. The recommended way to do this would be to use an ATC (normal) postP. Swap the heads via tool numbers. Head swap would be in each tool macro.

Example: T1 = Z head. That tool macro must include the following:
G53 (lifts all vertical axes)
G54
L12 ZW

Example: T2 = W head. That tool macro must include the following:
G53 (lifts all vertical axes)
G55 (defined in INI as offset for W head)
L12 WZ

This could be entered into as many tool macros as needed
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com

User avatar
Jim_in_PA
Vectric Apprentice
Posts: 162
Joined: Wed Jan 10, 2018 3:24 am
Model of CNC Machine: Camaster Stinger II SR-44 (MacOS user)

Re: "W" AXIS POST PROCESSOR

Post by Jim_in_PA »

I was thinking along the same lines as Gary after reading the OP. You may want to examine the Camaster X3 post processor in the Vectric software to see how they did things for their three spindle setup. Reading the file might be helpful and instructive. While I rarely make any changes to my system, I've found it very interesting and helpful to read through various files to better understand how things are setup to work.

User avatar
IslaWW
Vectric Wizard
Posts: 1303
Joined: Wed Nov 21, 2007 11:42 pm
Model of CNC Machine: The Ultimate Woodworking Machine
Location: Marquette, MI, USA

Re: "W" AXIS POST PROCESSOR

Post by IslaWW »

The system that operates the X-3 is a bit bastardized, so not so much help from the postP there. That said, there is good info to learn from the X-3 toolchange macros as they apply tool head offsets and switch on different cutting heads.
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com

User avatar
Jim_in_PA
Vectric Apprentice
Posts: 162
Joined: Wed Jan 10, 2018 3:24 am
Model of CNC Machine: Camaster Stinger II SR-44 (MacOS user)

Re: "W" AXIS POST PROCESSOR

Post by Jim_in_PA »

IslaWW wrote:
Tue Mar 24, 2020 6:47 pm
The system that operates the X-3 is a bit bastardized, so not so much help from the postP there. That said, there is good info to learn from the X-3 toolchange macros as they apply tool head offsets and switch on different cutting heads.
"Ah!" on the first part and "that's what I was thinking" on the second. :D

Post Reply