Need advise for PP with ATC

This forum is for requests and queries about machine tool support for Vectric Products

Need advise for PP with ATC

Postby Allen » Fri Mar 08, 2019 1:30 am

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
Allen
Vectric Apprentice
 
Posts: 18
Joined: Sat Oct 24, 2015 4:00 am
Model of CNC Machine: Built it myself/ Linuxcnc control

Re: Need advise for PP with ATC

Postby ger21 » Fri Mar 08, 2019 2:20 am

Something like this?

begin TOOLCHANGE

"[N]T[T]M6"
"[N] (Tool: [TOOLNAME])"
"[N]G43H[T]"
Gerry - http://www.thecncwoodworker.com
ger21
Vectric Wizard
 
Posts: 1314
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY

Re: Need advise for PP with ATC

Postby Allen » Fri Mar 08, 2019 4:55 pm

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
Allen
Vectric Apprentice
 
Posts: 18
Joined: Sat Oct 24, 2015 4:00 am
Model of CNC Machine: Built it myself/ Linuxcnc control

Re: Need advise for PP with ATC

Postby Allen » Fri Mar 15, 2019 3:00 am

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
Allen
Vectric Apprentice
 
Posts: 18
Joined: Sat Oct 24, 2015 4:00 am
Model of CNC Machine: Built it myself/ Linuxcnc control

Re: Need advise for PP with ATC

Postby Dan m » Fri Mar 15, 2019 3:39 am

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 m
 
Posts: 12
Joined: Sun Dec 16, 2018 11:31 pm
Model of CNC Machine: Router

Re: Need advise for PP with ATC

Postby Allen » Fri Mar 15, 2019 8:39 pm

Yes, I had to do a G53 in my configuration file on LCNC, it works though.

THX
Allen
Vectric Apprentice
 
Posts: 18
Joined: Sat Oct 24, 2015 4:00 am
Model of CNC Machine: Built it myself/ Linuxcnc control

Re: Need advise for PP with ATC

Postby Allen » Sat Mar 16, 2019 10:34 pm

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
%
Allen
Vectric Apprentice
 
Posts: 18
Joined: Sat Oct 24, 2015 4:00 am
Model of CNC Machine: Built it myself/ Linuxcnc control

Re: Need advise for PP with ATC

Postby IslaWW » Sun Mar 17, 2019 1:42 am

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?
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com
User avatar
IslaWW
Vectric Wizard
 
Posts: 1163
Joined: Wed Nov 21, 2007 11:42 pm
Location: Marquette, MI, USA
Model of CNC Machine: The Ultimate Woodworking Machine

Re: Need advise for PP with ATC

Postby Allen » Sun Mar 17, 2019 2:31 am

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]"
Allen
Vectric Apprentice
 
Posts: 18
Joined: Sat Oct 24, 2015 4:00 am
Model of CNC Machine: Built it myself/ Linuxcnc control

Re: Need advise for PP with ATC

Postby Allen » Sun Mar 17, 2019 9:40 pm

I have this sorted and working now,

Thank you.
Allen
Vectric Apprentice
 
Posts: 18
Joined: Sat Oct 24, 2015 4:00 am
Model of CNC Machine: Built it myself/ Linuxcnc control


Return to Post Processors

Who is online

Users browsing this forum: No registered users and 3 guests