Hi Folks,
I've been working through setting up a post for LinuxCNC with ATC, I have everything working as it should save one thing.
LinuxCNC allows you to "Touch off" your tools and records those results in the tool table, the height is recorded in the table as H(and tool number), that off set in my case would look like M6 G43 H? in the ngc code. I can't get the post to out put this line of code, I don't see anything in the "Post Processor Editing Guild" that detail this function.
Is this something Vectric will not provide for, or am I missing something?
Thank you in advance
Need advise for PP with ATC
-
- Vectric Wizard
- Posts: 1592
- Joined: Sun Sep 16, 2007 2:59 pm
- Model of CNC Machine: Custom DIY
- Location: Lake St Clair, MI, USA
- Contact:
Re: Need advise for PP with ATC
Something like this?
begin TOOLCHANGE
"[N]T[T]M6"
"[N] (Tool: [TOOLNAME])"
"[N]G43H[T]"
begin TOOLCHANGE
"[N]T[T]M6"
"[N] (Tool: [TOOLNAME])"
"[N]G43H[T]"
Gerry - http://www.thecncwoodworker.com
-
- Posts: 26
- Joined: Sat Oct 24, 2015 4:00 am
- Model of CNC Machine: Built it myself/ Linuxcnc control
Re: Need advise for PP with ATC
GER21,
Thanks for your help, that puts the call for the H offset in my ngc files, it's not where I'm accustom to seeing it, but the file loads and it is there.
I'll test this soon.
Thanks again
Thanks for your help, that puts the call for the H offset in my ngc files, it's not where I'm accustom to seeing it, but the file loads and it is there.
I'll test this soon.
Thanks again
-
- Posts: 26
- Joined: Sat Oct 24, 2015 4:00 am
- Model of CNC Machine: Built it myself/ Linuxcnc control
Re: Need advise for PP with ATC
I'm bewildered by an issue with locating my spindle in a good place for doing a manual tool change in a PP with ATC.
I have everything working as I would like, but it would be helpful if the spindle went to XH YH ZH to do the tool swap, can I put a G53 in the post? .
I have tried every VAR in the manual, when using the home position that's available to me, and then I try to load the ngc file, LCNC (my control OS) it errors me out with the old "Radius to end of arc differs from radius to start". (I really hate that one)
I have the required digits for Imperial (a common cause) so no worries there.
Can anyone give me some guidance on how I can do this?
Thanks for any help
I have everything working as I would like, but it would be helpful if the spindle went to XH YH ZH to do the tool swap, can I put a G53 in the post? .
I have tried every VAR in the manual, when using the home position that's available to me, and then I try to load the ngc file, LCNC (my control OS) it errors me out with the old "Radius to end of arc differs from radius to start". (I really hate that one)
I have the required digits for Imperial (a common cause) so no worries there.
Can anyone give me some guidance on how I can do this?
Thanks for any help
Re: Need advise for PP with ATC
On my controller its the tool change location is g28 but it's all done with my tool change macro the PP only calls out the m6 tool change and then the macro tells it what to do. I don't use Linux but I would assume it functions similar. You need to look for the macro file and edit it to call out your g28 tool change position.
Dan
Dan
-
- Posts: 26
- Joined: Sat Oct 24, 2015 4:00 am
- Model of CNC Machine: Built it myself/ Linuxcnc control
Re: Need advise for PP with ATC
Yes, I had to do a G53 in my configuration file on LCNC, it works though.
THX
THX
-
- Posts: 26
- Joined: Sat Oct 24, 2015 4:00 am
- Model of CNC Machine: Built it myself/ Linuxcnc control
Re: Need advise for PP with ATC
I was just running this test file for my PP and noticed something I can't explain or change, no mention of it in the manual either.
You will note there is a plunge rate on G01 under "Outside Profile" and under "Inside Profile" and "Line" the G01 has no plunge rate.
How do I get those plunge rates to load when I post the file?
%
(Vectric post test file File created: Saturday March 16 2019 - 02:27 PM)
G17 G20 G90 G40 G49 G64 P0.001
(Outside Profile)
T1 M06 (T1 End Mill 0.25 inch)
G43 H1
M03 S12000
G54 (Coordinate System)
G0 Z0.5000X1.0364Y3.3945
G0 Z0.2000
G01 Z-0.2500 F10.0000 G4 P0.5
G2X0.4114Y4.0195I0.0000J0.6250F52.2500
G2X1.0364Y4.6445I0.6250J0.0000
G2X1.6614Y4.0195I0.0000J-0.6250
G2X1.0364Y3.3945I-0.6250J0.0000
G0 Z0.5000
(Inside Profile)
M6 T21 (T21 End Mill 0.125 inch)
G43 H21
S12000 M03
G54 (Coordinate System)
G0 Z0.5000X3.3272Y1.3472
G0 Z0.2000
G01 Z-0.2500 G4 P0.5
G2X3.7647Y1.7847I0.4375J0.0000F52.0000
G2X4.2022Y1.3472I0.0000J-0.4375
G2X3.7647Y0.9097I-0.4375J0.0000
G2X3.3272Y1.3472I0.0000J0.4375
G0 Z0.5000
(Line)
M6 T1 (T1 End Mill 0.25 inch)
G43 H1
S12000 M03
G54 (Coordinate System)
G0 Z0.5000X1.4093Y2.6212
G0 Z0.2000
G01 Z-0.2500 G4 P0.5
G1X3.9449F52.2500
G0 Z0.5000
G0Z0.5010
G0X1.0000Y1.0000
M2
%
You will note there is a plunge rate on G01 under "Outside Profile" and under "Inside Profile" and "Line" the G01 has no plunge rate.
How do I get those plunge rates to load when I post the file?
%
(Vectric post test file File created: Saturday March 16 2019 - 02:27 PM)
G17 G20 G90 G40 G49 G64 P0.001
(Outside Profile)
T1 M06 (T1 End Mill 0.25 inch)
G43 H1
M03 S12000
G54 (Coordinate System)
G0 Z0.5000X1.0364Y3.3945
G0 Z0.2000
G01 Z-0.2500 F10.0000 G4 P0.5
G2X0.4114Y4.0195I0.0000J0.6250F52.2500
G2X1.0364Y4.6445I0.6250J0.0000
G2X1.6614Y4.0195I0.0000J-0.6250
G2X1.0364Y3.3945I-0.6250J0.0000
G0 Z0.5000
(Inside Profile)
M6 T21 (T21 End Mill 0.125 inch)
G43 H21
S12000 M03
G54 (Coordinate System)
G0 Z0.5000X3.3272Y1.3472
G0 Z0.2000
G01 Z-0.2500 G4 P0.5
G2X3.7647Y1.7847I0.4375J0.0000F52.0000
G2X4.2022Y1.3472I0.0000J-0.4375
G2X3.7647Y0.9097I-0.4375J0.0000
G2X3.3272Y1.3472I0.0000J0.4375
G0 Z0.5000
(Line)
M6 T1 (T1 End Mill 0.25 inch)
G43 H1
S12000 M03
G54 (Coordinate System)
G0 Z0.5000X1.4093Y2.6212
G0 Z0.2000
G01 Z-0.2500 G4 P0.5
G1X3.9449F52.2500
G0 Z0.5000
G0Z0.5010
G0X1.0000Y1.0000
M2
%
- IslaWW
- Vectric Wizard
- Posts: 1402
- Joined: Wed Nov 21, 2007 11:42 pm
- Model of CNC Machine: CNC Controller Upgrades
- Location: Bergland, MI, USA
Re: Need advise for PP with ATC
Where tou have the "F" parameter defined, are you using an "A" for all or "C" for when it changes?
Are you using a "first feed move " and a "feed move" and do the both have the [F] variable in them?
Are you using a "first feed move " and a "feed move" and do the both have the [F] variable in them?
Gary Campbell
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com
GCnC Control
ATC & Servo Controller Controller Upgrades
GCnC411 (at) gmail.com
-
- Posts: 26
- Joined: Sat Oct 24, 2015 4:00 am
- Model of CNC Machine: Built it myself/ Linuxcnc control
Re: Need advise for PP with ATC
Thanks for responding.
Hmm, I might see where you're going, here are some of the post var's.
VAR FEED_RATE = [F|C|F|1.4]
VAR CUT_RATE = [FC|C|F|1.4]
VAR PLUNGE_RATE = [FP|C|F|1.4]
+ ---------------------------------------------------
+ Commands output for First_PLUNGE Moves
+ ---------------------------------------------------
begin FIRST_PLUNGE_MOVE
"G01 [Z] [FP] G4 P0.5"
+ ---------------------------------------------------
+ Commands output for PLUNGE Moves
+ ---------------------------------------------------
begin PLUNGE_MOVE
"G01 [Z] [FP]"
+---------------------------------------------------
+ Commands output for the first feed rate move
+---------------------------------------------------
begin FIRST_FEED_MOVE
"G1[X][Y][Z][FC]"
+---------------------------------------------------
+ Commands output for feed rate moves
+---------------------------------------------------
begin FEED_MOVE
"G1[X][Y][Z]"
Hmm, I might see where you're going, here are some of the post var's.
VAR FEED_RATE = [F|C|F|1.4]
VAR CUT_RATE = [FC|C|F|1.4]
VAR PLUNGE_RATE = [FP|C|F|1.4]
+ ---------------------------------------------------
+ Commands output for First_PLUNGE Moves
+ ---------------------------------------------------
begin FIRST_PLUNGE_MOVE
"G01 [Z] [FP] G4 P0.5"
+ ---------------------------------------------------
+ Commands output for PLUNGE Moves
+ ---------------------------------------------------
begin PLUNGE_MOVE
"G01 [Z] [FP]"
+---------------------------------------------------
+ Commands output for the first feed rate move
+---------------------------------------------------
begin FIRST_FEED_MOVE
"G1[X][Y][Z][FC]"
+---------------------------------------------------
+ Commands output for feed rate moves
+---------------------------------------------------
begin FEED_MOVE
"G1[X][Y][Z]"
-
- Posts: 26
- Joined: Sat Oct 24, 2015 4:00 am
- Model of CNC Machine: Built it myself/ Linuxcnc control
Re: Need advise for PP with ATC
I have this sorted and working now,
Thank you.
Thank you.