Topics

Tool Change GCode

Yahoo
 

I just finished my first pcb board using pcb-gcode 3.6.2  and had a problem with the drill code.  In the pcb-gcode setup, I included the Tool Change position X= 5 Y= 0 Z= 1.5 to move the tool to the front center of my machine to make it easy to do a manual tool change.  I also have the work piece located near the center of the X axis of the machine.  When the code hits the tool change code

 

G00 Z1.5000

G00 X5.0000 Y0.0000

 

The machine moves 5” from the zero point of the material not from the machine coordinates.  Should the second line also include “G53” which would move to where I intend it move?  I would expect that the Tool Change position should not move because of the location of the material being worked on.

 

Is this a bug or do I not understand something?   I am not an expert by any means, so if someone out there can help with my education I will appreciate any help.

 

Thank you JJ for the great product.

Art Eckstein
 

Based on what you have said, YES you need to include the G53 as the program most likely is in G54 offset. So presently it is going to the point based on the offset origin it is presently working in. The other option is to base your tool change point on the G54 offset coordinates.


Art
Country Bubba

At 01:04 PM 4/25/2014, you wrote:


I just finished my first pcb board using pcb-gcode 3.6.2 and had a problem with the drill code. In the pcb-gcode setup, I included the Tool Change position X= 5 Y= 0 Z= 1.5 to move the tool to the front center of my machine to make it easy to do a manual tool change. I also have the work piece located near the center of the X axis of the machine. When the code hits the tool change code

G00 Z1.5000
G00 X5.0000 Y0.0000

The machine moves 5" from the zero point of the material not from the machine coordinates. Should the second line also include "G53" which would move to where I intend it move? I would expect that the Tool Change position should not move because of the location of the material being worked on.

Is this a bug or do I not understand something? I am not an expert by any means, so if someone out there can help with my education I will appreciate any help.

Thank you JJ for the great product.

casy_ch@tbwil.ch
 

To me as a cnc machine user the zero machine coordinates are just a reference for the machine and its electronic to know a basic position, then you forget about it unless you lost some steps which should not take place! Programming the G-Code is always done from the zero coordinates of the work piece to process the work. Up to you to find the coordinates you want based from the zero workpiece.

Represent yourself a paper drawing of the work piece and lay it on your machine. Everything you are thinking of is always related to the drawing.

Jean-Claude

Am 25.04.2014 19:04, schrieb Yahoo:

 

I just finished my first pcb board using pcb-gcode 3.6.2  and had a problem with the drill code.  In the pcb-gcode setup, I included the Tool Change position X= 5 Y= 0 Z= 1.5 to move the tool to the front center of my machine to make it easy to do a manual tool change.  I also have the work piece located near the center of the X axis of the machine.  When the code hits the tool change code

 

G00 Z1.5000

G00 X5.0000 Y0.0000

 

The machine moves 5” from the zero point of the material not from the machine coordinates.  Should the second line also include “G53” which would move to where I intend it move?  I would expect that the Tool Change position should not move because of the location of the material being worked on.

 

Is this a bug or do I not understand something?   I am not an expert by any means, so if someone out there can help with my education I will appreciate any help.

 

Thank you JJ for the great product.


Ward Elder
 

The problem with “tool change position” is it may relate to the physical machine.  I have an ATC so I need to reference to the machine coordinates not the work piece.  I would think that even on manual tool change a user would always want the tool change position to be in the same place regardless of the work piece location.

 

 

Thank you,

 

 

Ward M. Elder

Eldersoft

42 Appleton St.

Winnipeg, MB

R2G1K5

(204) 791-7754   (Cell)

ward@...

 

From: pcb-gcode@... [mailto:pcb-gcode@...] On Behalf Of casy_ch@...
Sent: Friday, April 25, 2014 12:22 PM
To: pcb-gcode@...
Subject: Re: [pcb-gcode] Tool Change GCode

 

 

To me as a cnc machine user the zero machine coordinates are just a reference for the machine and its electronic to know a basic position, then you forget about it unless you lost some steps which should not take place! Programming the G-Code is always done from the zero coordinates of the work piece to process the work. Up to you to find the coordinates you want based from the zero workpiece.

Represent yourself a paper drawing of the work piece and lay it on your machine. Everything you are thinking of is always related to the drawing.

Jean-Claude

Am 25.04.2014 19:04, schrieb Yahoo:

 

I just finished my first pcb board using pcb-gcode 3.6.2  and had a problem with the drill code.  In the pcb-gcode setup, I included the Tool Change position X= 5 Y= 0 Z= 1.5 to move the tool to the front center of my machine to make it easy to do a manual tool change.  I also have the work piece located near the center of the X axis of the machine.  When the code hits the tool change code

 

G00 Z1.5000

G00 X5.0000 Y0.0000

 

The machine moves 5” from the zero point of the material not from the machine coordinates.  Should the second line also include “G53” which would move to where I intend it move?  I would expect that the Tool Change position should not move because of the location of the material being worked on.

 

Is this a bug or do I not understand something?   I am not an expert by any means, so if someone out there can help with my education I will appreciate any help.

 

Thank you JJ for the great product.

 

Yahoo
 

I would agree with you completely when you are talking about the work piece, but here I am talking about where the tool change position is.  This does not change based on which position the piece is in (G54,G55,G56,…) The tool change is unchanging for a particular machine.

 

Where within the code is the Tool Change created?  I could manually change the line each time I create a drill file but I would rather change the program to remember that information.

 

 

From: pcb-gcode@... [mailto:pcb-gcode@...] On Behalf Of casy_ch@...
Sent: Friday, April 25, 2014 1:22 PM
To: pcb-gcode@...
Subject: Re: [pcb-gcode] Tool Change GCode

 

 

To me as a cnc machine user the zero machine coordinates are just a reference for the machine and its electronic to know a basic position, then you forget about it unless you lost some steps which should not take place! Programming the G-Code is always done from the zero coordinates of the work piece to process the work. Up to you to find the coordinates you want based from the zero workpiece.

Represent yourself a paper drawing of the work piece and lay it on your machine. Everything you are thinking of is always related to the drawing.

Jean-Claude

Am 25.04.2014 19:04, schrieb Yahoo:

 

I just finished my first pcb board using pcb-gcode 3.6.2  and had a problem with the drill code.  In the pcb-gcode setup, I included the Tool Change position X= 5 Y= 0 Z= 1.5 to move the tool to the front center of my machine to make it easy to do a manual tool change.  I also have the work piece located near the center of the X axis of the machine.  When the code hits the tool change code

 

G00 Z1.5000

G00 X5.0000 Y0.0000

 

The machine moves 5” from the zero point of the material not from the machine coordinates.  Should the second line also include “G53” which would move to where I intend it move?  I would expect that the Tool Change position should not move because of the location of the material being worked on.

 

Is this a bug or do I not understand something?   I am not an expert by any means, so if someone out there can help with my education I will appreciate any help.

 

Thank you JJ for the great product.

 


No virus found in this message.
Checked by AVG - www.avg.com
Version: 2014.0.4570 / Virus Database: 3920/7393 - Release Date: 04/25/14

Art Eckstein
 

On my pcb machine, I generally use THREE different offsets:
1. G53 because this is where I tell the spindle to go for tool changes and automatic tool length measurement.
2. G54 which is used as the coordinates system for working on the bottom side of the pcb
3. G55 which is used for the top side of the pcb.

By doing this, I have one fixture and turn the board over in the exact same place. Of course this changes the origin location with respect to the fixture, but is the same place on the board.

This was easily accomplished by customizing my post processor to the required offsets and doing the tool touch off.

At 01:21 PM 4/25/2014, you wrote:


To me as a cnc machine user the zero machine coordinates are just a reference for the machine and its electronic to know a basic position, then you forget about it unless you lost some steps which should not take place! Programming the G-Code is always done from the zero coordinates of the work piece to process the work. Up to you to find the coordinates you want based from the zero workpiece.

Represent yourself a paper drawing of the work piece and lay it on your machine. Everything you are thinking of is always related to the drawing.

Jean-Claude

Am 25.04.2014 19:04, schrieb Yahoo:


I just finished my first pcb board using pcb-gcode 3.6.2 and had a problem with the drill code. In the pcb-gcode setup, I included the Tool Change position X= 5 Y= 0 Z= 1.5 to move the tool to the front center of my machine to make it easy to do a manual tool change. I also have the work piece located near the center of the X axis of the machine. When the code hits the tool change code



G00 Z1.5000

G00 X5.0000 Y0.0000



The machine moves 5" from the zero point of the material not from the machine coordinates. Should the second line also include "G53" which would move to where I intend it move? I would expect that the Tool Change position should not move because of the location of the material being worked on.



Is this a bug or do I not understand something? I am not an expert by any means, so if someone out there can help with my education I will appreciate any help.



Thank you JJ for the great product.

John Johnson <pcbgcode@...>
 

You can change how the g-code is generated in settings/gcode-defaults.h
If there is something more specialized you need to do, you can look into adding code for user g-gcode. I'd start with settings/gcode-defaults.h first. When you have the code working, be sure and copy settings/gcode-defaults.h to profiles/yourmachine.pp so if you change profiles for some reason, you'll be able to change back. (The .pp files are copied to gcode-defaults.h when you select your g-code style when setting the program up.)

Regards,
JJ


On Fri, Apr 25, 2014 at 1:34 PM, Art Eckstein <art.eckstein@...> wrote:
 

On my pcb machine, I generally use THREE different offsets:
1. G53 because this is where I tell the spindle to go for tool
changes and automatic tool length measurement.
2. G54 which is used as the coordinates system for working on the
bottom side of the pcb
3. G55 which is used for the top side of the pcb.

By doing this, I have one fixture and turn the board over in the
exact same place. Of course this changes the origin location with
respect to the fixture, but is the same place on the board.

This was easily accomplished by customizing my post processor to the
required offsets and doing the tool touch off.



At 01:21 PM 4/25/2014, you wrote:

>To me as a cnc machine user the zero machine coordinates are just a
>reference for the machine and its electronic to know a basic
>position, then you forget about it unless you lost some steps which
>should not take place! Programming the G-Code is always done from
>the zero coordinates of the work piece to process the work. Up to
>you to find the coordinates you want based from the zero workpiece.
>
>Represent yourself a paper drawing of the work piece and lay it on
>your machine. Everything you are thinking of is always related to the drawing.
>
>Jean-Claude
>
>Am 25.04.2014 19:04, schrieb Yahoo:
>>
>>
>>I just finished my first pcb board using pcb-gcode 3.6.2 and had a
>>problem with the drill code. In the pcb-gcode setup, I included
>>the Tool Change position X= 5 Y= 0 Z= 1.5 to move the tool to the
>>front center of my machine to make it easy to do a manual tool
>>change. I also have the work piece located near the center of the
>>X axis of the machine. When the code hits the tool change code
>>
>>
>>
>>G00 Z1.5000
>>
>>G00 X5.0000 Y0.0000
>>
>>
>>
>>The machine moves 5" from the zero point of the material not from
>>the machine coordinates. Should the second line also include "G53"
>>which would move to where I intend it move? I would expect that
>>the Tool Change position should not move because of the location of
>>the material being worked on.
>>
>>
>>
>>Is this a bug or do I not understand something? I am not an
>>expert by any means, so if someone out there can help with my
>>education I will appreciate any help.
>>
>>
>>
>>Thank you JJ for the great product.




--
Sent from a MacBook Pro