Creating Multiple Tool G-Codes in Torchmate CAD/CAM (Lite too!) - Pirate4x4.Com : 4x4 and Off-Road Forum
 
Pirate4x4.Com : 4x4 and Off-Road Forum  

Go Back   Pirate4x4.Com : 4x4 and Off-Road Forum > Vendor Forums > Torchmate CNC Forum
Notices

 
 
Share LinkBack Thread Tools Display Modes
Old 09-04-2012, 09:44 AM   #1 (permalink)
Registered User
 
Join Date: Jan 2010
Member # 152411
Location: Reno NV
Posts: 777
Creating Multiple Tool G-Codes in Torchmate CAD/CAM (Lite too!)

I just wanted to take a minute and post a way to create a g-code file directly from Torchmate CAD that contains all of the tool changes, cut order, and offsets necessary to run a multiple tool g-code in the Torchmate driver software. This method is called Machine Output

This method has been tested with version 8 of Torchmate CAD/CAM (or Lite) and Version 4 of the Torchmate Driver Software. Other version may have a few errors in the g-code or execution of the g-code.

This method requires some advanced Torchmate CAD knowledge such as cut sequencing and creating multiple tool paths within the same file. Torchmate technical support is always available to answer questions. Please file this under an advanced method and not something that I would recommend that someone just learning the basics not try this yet as there can be some confusion created.

I, or someone in technical support, will be creating a video soon on this method as well.

To begin you will need to set up a few things in Torchmate CAD.
Go to Machine > Machining Defaults
Under "Selected Driver" choose Torchmate Dual Tool Driver
In this menu also be sure that:
Material and Selected are checked under "Machining"
Multi-tool is selected under "Tool"
Also if your table is larger than eight feet in any dimension select the Setup button and in this menu enter your table size under Machine Limits. (This is not too critical for smaller tables as this just establishes an upper limit of part size for a table, but any size may be entered if you'd like a secondary check of part sizing)

Press Apply and Close in this menu.

Using this method all aspects of the cut need to be set in Torchmate CAD/CAM. This includes the tool number and feedrate.

Ensure that the feedrates in Torchmate CAD match those in the driver software. Go to Options > Torchmate Setup > General Preferences and select in/min for "speed units".

To edit the tool number go to Machine > Tool Library

For each tool in your library there are a few parameters than can be set, in the past only the D1 value mattered as this was the offset the CAD used when creating the toolpath. When using machine output another parameter that is necessary is the turret number. The turret number corresponds to the tool number in the Torchmate Driver software. For instance if your plasma is considered tool #1 in the Torchmate driver software then in Torchmate CAD the turret number must be 1. If your plate marker is tool #2 in the driver software it must be turret 2 in CAD.

Change your tool library to reflect the tool setup in your driver software.

------------------------------------------------------------------------

At this point we want to create a test file that walks through a multiple tool part. A basic shape of a marked circle inside of a cutout square will be described here.

Draw the two objects as you normally would, do not make a path on both objects as they need to remain two separate pieces.

When using machine output the rulers in Torchmate CAD are also the program coordinates in the driver software so if you want the lower left corner to be at (0,0) in the driver software move the corner of the square to that position in Torchmate CAD.

Select the circle (plate marker) and go to Machine > Create Toolpath > Online

In the Basic Cut tab select the plate marker tool you created with the correct turret. In this tab you must also specify the feed rate.

Create a tool path for the square in the same manner (use a male tool path for the cutout) Ensure that in the Basic Cut tab the plasma tool with the correct turret number is selected and a feed rate is specified for the plasma. You create lead ins/outs the same as normal.

------------------------------------------------------------------------

At this point you should have two separate tool paths and the original objects as well. The objects need to be sequenced so that the plate marker circle is done before the cut out square. Multiple ways exist to sequence parts and on complex or involved parts some methods are better than others.

For two simple objects I use the tool path viewer.

Go to View > Show Tool Path Viewer
Check the Show Order check box

This displays a number next to the start of each tool path that corresponds to the order the machine will cut. To change the order double click on the tool path and a To Position window will appear and you can type in the place in the cut order you want that part cut.

For this simple part make sure that a 1 is next to the circle and a 2 is next to the square.

------------------------------------------------------------------------

At this point the part is ready to be converted to a g-code. A few things to be aware of when processing.

-The g-code will only be created for tool paths, other objects are ignored.
-Any tool path outside of the material size will be ignored, ensure that the entire tool path is within the material (even the lead in).
-Only selected tool paths will be converted, if it is not selected it will be ignored.

To create the g-code go to Machine > Output

A new window will appear called "Cut Preview" This will show the material size and the tool paths that are to be converted to g-code. For the sake of this guide I will just say that there are many fancy things that can be done in here but if you want to just cut the part as you have drawn it select the last icon on the little tool bar that appears (it looks like scissors and if you mouse over it the name is "Machining") .

There will now be a save dialog to save the g-code.

This g-code contains all of the tool changes, offset changes, feedrates, and cut order.

You just need to open the g-code in the Torchmate Driver software, zero and cut.

Like I said, this is fairly advanced, a video is coming, and if you have any questions contact Torchmate support. I would also suggest creating a few simple shapes and simulating them in the driver software to get a feel for this method.

-Jack
__________________
Torchmate Technical Support - 6 AM to 4 PM PST
866-571-1066 x59221
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
TorchmateSupport is offline   Quick reply to this message
Old 09-04-2012, 10:11 AM   #2 (permalink)
Registered User
 
Join Date: Mar 2009
Member # 132992
Posts: 1,668
Very cool! I thought when I saw that you could assign a Turret to the tools that something like this could be done. Testing it out now.
__________________

To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
-- Jeffrey R Holland

Link:
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

I know it. I live it. I love it!


To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
jdh239 is offline   Quick reply to this message
Old 09-04-2012, 10:16 AM   #3 (permalink)
Registered User
 
Join Date: Mar 2009
Member # 132992
Posts: 1,668
A couple of issues I have found so far:

1. If you delete your regulart non-toolpath objects, you wont be able to do anything under machining > output. Keep those in there and you can get into it.

2. When I try to click on the scissors (machining) option, I get a brief message saying something about sending zero bytes to com1. Nothing that allows me to save the gcode out.

If you have a recommendation for number 2 above, that would be great.... otherwise I will just keep plugging away at it to see if I can get it to work.
__________________

To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
-- Jeffrey R Holland

Link:
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

I know it. I live it. I love it!


To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

Last edited by jdh239; 09-04-2012 at 10:18 AM.
jdh239 is offline   Quick reply to this message
Old 09-04-2012, 10:17 AM   #4 (permalink)
Registered User
 
Join Date: Jan 2010
Member # 152411
Location: Reno NV
Posts: 777
I forgot to mention one thing. Torchmate CAD/CAM uses M50 for tool on and M51 for tool off. Depending on the way your specific Torchmate driver software is setup you may need to make some changes.

For example just opening a default growth series setup file the following changes would need to be made in the driver software.

Go to Configuration > Programming > M-Code Definitions
Change the M-Code for Plasma On from 50 to 20
Change the M-Code for Plasma Off from 51 to 21
Delete the entire Plasma only macro previously listed as M20
Change the M-Code for Multi Tool Start from 22 to 50
Change the M-Code for Mutli Tool Stop from 23 to 51

Also click Macro for Multi Tool Start and edit it so that this line:

ELSEIF #CURRTOOL = 1 THEN
M50
M101 I1 "No Pierce Signal From AVHC"

becomes this line:

ELSEIF #CURRTOOL = 1 THEN
M20
M101 I1 "No Pierce Signal From AVHC"

Click OK

Then click Macro for Multi Tool Start and edit it so that this line:

ELSEIF #CURRTOOL = 1 THEN
M51

Becomes this:

ELSEIF #CURRTOOL = 1 THEN
M21


Under Configuration > Programming > M-Code Execution change Feedrate Move to 50 and All Other Times to 51 to match the multi tool commands in the definitions.
------------------------------------------------

Essentially if your setup file is different that the default 50 and 51 need to be the multi-tool activation commands and plasma on/off must be something else and the macros need to be updated to reflect this.

Please ask questions, technical support can help. If you are confused or need help please ask.

Video will be coming soon on the complete setup.

-Jack
__________________
Torchmate Technical Support - 6 AM to 4 PM PST
866-571-1066 x59221
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

Last edited by TorchmateSupport; 09-04-2012 at 11:29 AM.
TorchmateSupport is offline   Quick reply to this message
Old 09-04-2012, 10:23 AM   #5 (permalink)
Registered User
 
Join Date: Jan 2010
Member # 152411
Location: Reno NV
Posts: 777
Quote:
Originally Posted by jdh239 View Post
2. When I try to click on the scissors (machining) option, I get a brief message saying something about sending zero bytes to com1. Nothing that allows me to save the gcode out.

If you have a recommendation for number 2 above, that would be great.... otherwise I will just keep plugging away at it to see if I can get it to work.
Go to Machine > Machining Defaults

Click on setup next to the selected driver

There will be a menu with three tabs. Under the Port tab for "Port Location" select FILE: this should solve the issue.

Be sure to apply before closing.

Be sure that the Torchmate Dual Tool Driver is selected as well.

Let me know if this doesn't solve the issue.
-Jack
__________________
Torchmate Technical Support - 6 AM to 4 PM PST
866-571-1066 x59221
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
TorchmateSupport is offline   Quick reply to this message
Old 09-04-2012, 10:38 AM   #6 (permalink)
Registered User
 
Join Date: Mar 2009
Member # 132992
Posts: 1,668
Quote:
Originally Posted by TorchmateSupport View Post
Go to Machine > Machining Defaults

Click on setup next to the selected driver

There will be a menu with three tabs. Under the Port tab for "Port Location" select FILE: this should solve the issue.

Be sure to apply before closing.

Be sure that the Torchmate Dual Tool Driver is selected as well.

Let me know if this doesn't solve the issue.
-Jack
Awesome, that was it (and the Torchmate Dual Tool Driver). I will go and tweak my macros now to see if the other errors I am getting go away.
__________________

To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
-- Jeffrey R Holland

Link:
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

I know it. I live it. I love it!


To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
jdh239 is offline   Quick reply to this message
Old 09-04-2012, 10:46 AM   #7 (permalink)
Registered User
 
Join Date: Mar 2009
Member # 132992
Posts: 1,668
I am getting M codes 54 and 55 when I export from TM CAD, which of course are unrecognized:

G90
M06 T2
G43 H2
G00 X2.276 Y1.816
M54

G02 X1.4474 Y2.6440 I-0.0000 J0.8285
G02 X2.2759 Y3.4725 I0.8285 J0.0000
G02 X3.1044 Y2.6440 I0.0000 J-0.8285
G02 X2.2759 Y1.8156 I-0.8285 J-0.0000
G02 X1.4474 Y2.6440 I-0.0000 J0.8285
G02 X2.2759 Y3.4725 I0.8285 J0.0000
G02 X3.1044 Y2.6440 I0.0000 J-0.8285
G02 X2.2759 Y1.8156 I-0.8285 J-0.0000
G02 X1.4474 Y2.6440 I-0.0000 J0.8285
G02 X2.2759 Y3.4725 I0.8285 J0.0000
G02 X3.1044 Y2.6440 I0.0000 J-0.8285
G02 X2.2759 Y1.8156 I-0.8285 J-0.0000
M55

G00 X0.000 Y0.000
M02
__________________

To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
-- Jeffrey R Holland

Link:
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

I know it. I live it. I love it!


To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
jdh239 is offline   Quick reply to this message
Old 09-04-2012, 11:01 AM   #8 (permalink)
Registered User
 
Join Date: Mar 2009
Member # 132992
Posts: 1,668
Posting all this info here in case others need to reference it. Looks right to me, but let me know if I have something misconfigured:
Attached Images
  
__________________

To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
-- Jeffrey R Holland

Link:
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

I know it. I live it. I love it!


To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
jdh239 is offline   Quick reply to this message
Old 09-04-2012, 11:20 AM   #9 (permalink)
Registered User
 
Join Date: Jan 2007
Member # 84593
Location: Reno, NV
Posts: 4,236
Send a message via AIM to HardcorewannabeXJ Send a message via MSN to HardcorewannabeXJ
Quote:
Originally Posted by jdh239 View Post
I am getting M codes 54 and 55 when I export from TM CAD, which of course are unrecognized:

G90
M06 T2
G43 H2
G00 X2.276 Y1.816
M54

G02 X1.4474 Y2.6440 I-0.0000 J0.8285
G02 X2.2759 Y3.4725 I0.8285 J0.0000
G02 X3.1044 Y2.6440 I0.0000 J-0.8285
G02 X2.2759 Y1.8156 I-0.8285 J-0.0000
G02 X1.4474 Y2.6440 I-0.0000 J0.8285
G02 X2.2759 Y3.4725 I0.8285 J0.0000
G02 X3.1044 Y2.6440 I0.0000 J-0.8285
G02 X2.2759 Y1.8156 I-0.8285 J-0.0000
G02 X1.4474 Y2.6440 I-0.0000 J0.8285
G02 X2.2759 Y3.4725 I0.8285 J0.0000
G02 X3.1044 Y2.6440 I0.0000 J-0.8285
G02 X2.2759 Y1.8156 I-0.8285 J-0.0000
M55

G00 X0.000 Y0.000
M02
The M-codes that you get depend on the Tool Type on the tool library screen. Set ALL tools to the Plasma type and you will get m50 and m51 codes from CAD. When you change the type to something else you will get different on and off m-codes.
HardcorewannabeXJ is offline   Quick reply to this message
Old 09-04-2012, 11:24 AM   #10 (permalink)
Registered User
 
Join Date: Jan 2010
Member # 152411
Location: Reno NV
Posts: 777
Quote:
Originally Posted by jdh239 View Post
I am getting M codes 54 and 55 when I export from TM CAD, which of course are unrecognized:
Like Mike said above,

What type of tool is your plasma in the Torchmate CAD/CAM tool library?

Go to Machine >Tool Library, the middle section is the tool type.

This type affects what M-codes are used. In your case you may have it as an end-mill type.

If the type is "Plasma" the commands will be 50 and 51. Other tool types will use different commands. "Marker" uses 52 and 53. "End Mill" uses 54 and 55.

What ever type you use make sure that it is the same for all turrets and that your m-codes match in the driver software
__________________
Torchmate Technical Support - 6 AM to 4 PM PST
866-571-1066 x59221
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

Last edited by TorchmateSupport; 09-04-2012 at 11:25 AM.
TorchmateSupport is offline   Quick reply to this message
Old 09-04-2012, 11:27 AM   #11 (permalink)
Registered User
 
Join Date: Jan 2010
Member # 152411
Location: Reno NV
Posts: 777
Jon,
You will also want to change your m-Code execution numbers to match the changes made in the definitions section.

ie.
Change the mode to Full
Change the Feedrate Move to 50
Change the All Other Times to 51

I edited the above post to mention this as well.
-Jack
__________________
Torchmate Technical Support - 6 AM to 4 PM PST
866-571-1066 x59221
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

Last edited by TorchmateSupport; 09-04-2012 at 11:32 AM.
TorchmateSupport is offline   Quick reply to this message
Old 09-04-2012, 11:50 AM   #12 (permalink)
Registered User
 
Join Date: Mar 2009
Member # 132992
Posts: 1,668
Quote:
Originally Posted by TorchmateSupport View Post
Like Mike said above,

What type of tool is your plasma in the Torchmate CAD/CAM tool library?

Go to Machine >Tool Library, the middle section is the tool type.

This type affects what M-codes are used. In your case you may have it as an end-mill type.

If the type is "Plasma" the commands will be 50 and 51. Other tool types will use different commands. "Marker" uses 52 and 53. "End Mill" uses 54 and 55.

What ever type you use make sure that it is the same for all turrets and that your m-codes match in the driver software
I am getting a 55, but don't even have an endmill defined. Also, is there a place to enter default feedrates for tools?

Is there a list of default Mcodes somewhere I can look at?
__________________

To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
-- Jeffrey R Holland

Link:
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

I know it. I live it. I love it!


To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
jdh239 is offline   Quick reply to this message
Old 09-04-2012, 11:56 AM   #13 (permalink)
Registered User
 
Join Date: Mar 2009
Member # 132992
Posts: 1,668
seems like m54 and 55 are start/stop for the marker. In TM CAD I have "marker" as the tool set for my plate marker
__________________

To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
-- Jeffrey R Holland

Link:
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

I know it. I live it. I love it!


To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
jdh239 is offline   Quick reply to this message
Old 09-04-2012, 12:33 PM   #14 (permalink)
Registered User
 
Join Date: Jan 2010
Member # 152411
Location: Reno NV
Posts: 777
You could specify a feed rate and update the cut template, this would save it under the material thickness, tool path type (male, female, online), tool, all basic cut settings, lead in/out settings. If you move your files between computers you may run into conflicts if the cut templates on one computer don't match another, so be careful. Same goes for older files referencing the same cut template that has since been updated.

As far as the M numbers I would strongly suggest making all of the tool types plasma as this will ensure that 50 and 51 are your on and off commands.

Machine output can be used for single tool cutting as well and having all of your tools execute the same macro, then the turret to specify the tool number allows the macro in the driver software to take both these pieces and activate the correct tool. You could use other numbers it makes no performance difference, but from a support standpoint I'll recommend that 50 and 51 be used as this is what our crew will be expecting and it can avoid unnecessary confusion when speaking to them.

-Jack
__________________
Torchmate Technical Support - 6 AM to 4 PM PST
866-571-1066 x59221
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

Last edited by TorchmateSupport; 09-04-2012 at 12:36 PM.
TorchmateSupport is offline   Quick reply to this message
Old 09-04-2012, 01:34 PM   #15 (permalink)
Registered User
 
Join Date: Apr 2007
Member # 89324
Posts: 494
Very very interesting, I'm definitely going to be trying this out shortly. Can't wait to see the vid as well!
Conrad_Turbo is offline   Quick reply to this message
Old 09-04-2012, 02:15 PM   #16 (permalink)
Registered User
 
Join Date: Jan 2007
Member # 84593
Location: Reno, NV
Posts: 4,236
Send a message via AIM to HardcorewannabeXJ Send a message via MSN to HardcorewannabeXJ
Quote:
Originally Posted by jdh239 View Post
seems like m54 and 55 are start/stop for the marker. In TM CAD I have "marker" as the tool set for my plate marker
Right, you'll want to change this to Plasma as the type. The tool Type defines the m codes output from the CAD software, not the tool selection which is what Turret defines. Tool type should be set to Plasma for ALL tools regardless of what they actually are.
HardcorewannabeXJ is offline   Quick reply to this message
Old 11-29-2012, 11:07 AM   #17 (permalink)
Registered User
 
Join Date: Mar 2009
Member # 132992
Posts: 1,668
Question..... I was getting ready to put together another video with this, but when I highlight my plate marker and plasma tool paths and go to MACHINE > OUTPUT I only see the plate marker tool paths and not the plasma..... can't seem to figure out why yet.
__________________

To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
-- Jeffrey R Holland

Link:
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

I know it. I live it. I love it!


To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
jdh239 is offline   Quick reply to this message
Old 11-29-2012, 11:16 AM   #18 (permalink)
Registered User
 
Join Date: Mar 2009
Member # 132992
Posts: 1,668
Never mind... called TM support and they said that if it isn't showing up that the part isn't completely on the table (as set by the bounds). I moved it ontot the table (was barely off) and both tool paths show up now.
__________________

To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
-- Jeffrey R Holland

Link:
To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.

I know it. I live it. I love it!


To view links or images in signatures your post count must be 10 or greater. You currently have 0 posts.
jdh239 is offline   Quick reply to this message
Old 11-30-2012, 09:32 AM   #19 (permalink)
Registered User
 
Join Date: Sep 2002
Member # 13655
Location: Redstone Canyon, CO
Posts: 2,010
Quote:
Originally Posted by jdh239 View Post
Never mind... called TM support and they said that if it isn't showing up that the part isn't completely on the table (as set by the bounds). I moved it ontot the table (was barely off) and both tool paths show up now.
I actually like this "feature". It means I do not have to delete all my drawings when tooling, I just move them off the area defined as the table.

Perhaps TM support can elaborate on all the cool features shown in the interim Machine Output screen. Currently I am only using the scissors (Machining) option. Way cool.
__________________
89 XJ, 8" lift, 38's, locked F&R
98 LR Discovery - street poser
99 F350 PSD 4x4 Jeep Tow Truck
2003 Mini Cooper S - street go-kart
2004 Subaru WRX STi - Vette eater
2005 Mini Cooper S - street go-kart on LSD
Pile of tube, 383 SBC, and some buggy plans
XtremeJ is offline   Quick reply to this message
Old 11-30-2012, 10:21 AM   #20 (permalink)
Registered User
 
Join Date: Apr 2007
Member # 89324
Posts: 494
For guys with a Growth Series 4x4 table with plasma and a plate marker, can TM release a .stp configuration file that would set up all this these tooling changes and definitions? Then all we would have to do is update the TM CAD portion?

I am trying this offline and it's not quite cooperating. I would think releasing a .stp file to get people started along with a video would be a cheap investment to save hours of tech support time.
Conrad_Turbo is offline   Quick reply to this message
Old 12-02-2012, 02:42 PM   #21 (permalink)
Registered User
 
Join Date: Nov 2011
Member # 203032
Posts: 11
+1 on the included setup files for multiple tool setup(on a 2x2 though for me). I knew programming years ago when I owned a Commodore Vic20, but that thing is worm food now along with the programming portion of my brain.
skilawyer is offline   Quick reply to this message
Old 12-02-2012, 09:04 PM   #22 (permalink)
Registered User
 
Join Date: Nov 2011
Member # 203032
Posts: 11
I've been over and over this and I cant get my problem fixed.

I have the plate-marker set to move first, which it does, but the plasma fires at the same time. Sometimes i get the error trip message and the plate-marker keeps going despite pushing feed hold, and I have to switch off the control box. Any idea what i messed up?

this is my macro 50

IF #CURRTOOL = 0 THEN
M00 "NO TOOL SELECTED"
ELSEIF #CURRTOOL = 1 THEN
M20
ELSEIF #CURRTOOL = 2 THEN
M52
ELSE
M00 "NO TOOL SELECTED"
ENDIF

This is my macro 51

IF #CURRTOOL = 0 THEN
M00 "NO TOOL SELECTED"
ELSEIF #CURRTOOL = 1 THEN
M21
ELSEIF #CURRTOOL = 2 THEN
M53
ELSE
M00 "NO TOOL SELECTED"
ENDIF

This is macro 31

M06 T1
G43 H1

This is macro 32

M06 T2
G43 H2

Plasma on is 20, plasma off is 21.
Marker on is 52, marker off is 53.
All off is 59

Execution is set to full. Move 50, all other 51.
Safety trip/feed hold 59.

Turrets are defined in cad as plasma t1 and plasma(plate-marker) t2.
I set priority of plasma(plate-marker) t2 as first priority and plasma t1 as second priority.

Here are the first few lines of the g-code i am running.

G90
M06 T2
G43 H2
G00 X2.198 Y1.302
M50

G01 X2.251 Y1.302 F30.000
G02 X2.2659 Y1.3002 I0.0010 J-0.0644
G02 X2.2855 Y1.2835 I-0.0050 J-0.0258
G02 X2.2782 Y1.2557 I-0.0238 J-0.0085
G02 X2.2737 Y1.2526 I-0.0120 J0.0127
G02 X2.2541 Y1.2479 I-0.0209 J0.0439
G02 X2.1981 Y1.2477 I-0.0322 J1.0767
G01 X2.198 Y1.302
M51

G00 X2.198 Y1.302
G00 X2.197 Y1.149
M50

G01 X2.175 Y1.149 F30.000
G01 X2.175 Y1.320
G01 X2.250 Y1.320
G02 X2.2753 Y1.3182 I0.0041 J-0.1109
G02 X2.2862 Y1.3147 I-0.0128 J-0.0594
G02 X2.3041 Y1.2994 I-0.0124 J-0.0326
G02 X2.3050 Y1.2502 I-0.0400 J-0.0253
G02 X2.2964 Y1.2395 I-0.0324 J0.0173
G02 X2.2632 Y1.2266 I-0.0377 J0.0479
G02 X2.2784 Y1.2167 I-0.0233 J-0.0522
G02 X2.2956 Y1.1953 I-0.0805 J-0.0826
G01 X2.325 Y1.149
G01 X2.297 Y1.149
G03 X2.2578 Y1.2080 I-0.7673 J-0.4625
G03 X2.2500 Y1.2165 I-0.0502 J-0.0382
G03 X2.2306 Y1.2246 I-0.0201 J-0.0209
G03 X2.1972 Y1.2248 I-0.0203 J-0.6736
G01 X2.197 Y1.149
M51

Thanks in advance for the help!

12:33 am update- changed from full to basic with 50 on and 59 all other and it works.

Last edited by skilawyer; 12-02-2012 at 11:33 PM.
skilawyer is offline   Quick reply to this message
Old 12-03-2012, 09:51 AM   #23 (permalink)
Registered User
 
Join Date: Jan 2007
Member # 84593
Location: Reno, NV
Posts: 4,236
Send a message via AIM to HardcorewannabeXJ Send a message via MSN to HardcorewannabeXJ
Quote:
Originally Posted by skilawyer View Post
I've been over and over this and I cant get my problem fixed.

I have the plate-marker set to move first, which it does, but the plasma fires at the same time. Sometimes i get the error trip message and the plate-marker keeps going despite pushing feed hold, and I have to switch off the control box. Any idea what i messed up?

this is my macro 50

IF #CURRTOOL = 0 THEN
M00 "NO TOOL SELECTED"
ELSEIF #CURRTOOL = 1 THEN
M20
ELSEIF #CURRTOOL = 2 THEN
M52
ELSE
M00 "NO TOOL SELECTED"
ENDIF

This is my macro 51

IF #CURRTOOL = 0 THEN
M00 "NO TOOL SELECTED"
ELSEIF #CURRTOOL = 1 THEN
M21
ELSEIF #CURRTOOL = 2 THEN
M53
ELSE
M00 "NO TOOL SELECTED"
ENDIF

This is macro 31

M06 T1
G43 H1

This is macro 32

M06 T2
G43 H2

Plasma on is 20, plasma off is 21.
Marker on is 52, marker off is 53.
All off is 59

Execution is set to full. Move 50, all other 51.
Safety trip/feed hold 59.

Turrets are defined in cad as plasma t1 and plasma(plate-marker) t2.
I set priority of plasma(plate-marker) t2 as first priority and plasma t1 as second priority.

Here are the first few lines of the g-code i am running.

G90
M06 T2
G43 H2
G00 X2.198 Y1.302
M50

G01 X2.251 Y1.302 F30.000
G02 X2.2659 Y1.3002 I0.0010 J-0.0644
G02 X2.2855 Y1.2835 I-0.0050 J-0.0258
G02 X2.2782 Y1.2557 I-0.0238 J-0.0085
G02 X2.2737 Y1.2526 I-0.0120 J0.0127
G02 X2.2541 Y1.2479 I-0.0209 J0.0439
G02 X2.1981 Y1.2477 I-0.0322 J1.0767
G01 X2.198 Y1.302
M51

G00 X2.198 Y1.302
G00 X2.197 Y1.149
M50

G01 X2.175 Y1.149 F30.000
G01 X2.175 Y1.320
G01 X2.250 Y1.320
G02 X2.2753 Y1.3182 I0.0041 J-0.1109
G02 X2.2862 Y1.3147 I-0.0128 J-0.0594
G02 X2.3041 Y1.2994 I-0.0124 J-0.0326
G02 X2.3050 Y1.2502 I-0.0400 J-0.0253
G02 X2.2964 Y1.2395 I-0.0324 J0.0173
G02 X2.2632 Y1.2266 I-0.0377 J0.0479
G02 X2.2784 Y1.2167 I-0.0233 J-0.0522
G02 X2.2956 Y1.1953 I-0.0805 J-0.0826
G01 X2.325 Y1.149
G01 X2.297 Y1.149
G03 X2.2578 Y1.2080 I-0.7673 J-0.4625
G03 X2.2500 Y1.2165 I-0.0502 J-0.0382
G03 X2.2306 Y1.2246 I-0.0201 J-0.0209
G03 X2.1972 Y1.2248 I-0.0203 J-0.6736
G01 X2.197 Y1.149
M51

Thanks in advance for the help!

12:33 am update- changed from full to basic with 50 on and 59 all other and it works.
What version of the Torchmate Driver's software are you running? If you are running Version 3, you have to have it in the Basic mode. If you are in Version 4, you should be able to run it in Full executions. Based on all your settings listed, I would imagine you are in Version 3.

When you have a Code for the Start (After Hold) on Basic, keep in mind the tool will fire regardless of it's position on the table. This means if you pause in a rapid travel, and start again, it will cut/mark the rapid travel. I recommend leaving this option blank, and if you have to start in the middle of a cut or mark line, turn the tool on from the auxiliary menu, and then g-code start quickly after.

-Mike
HardcorewannabeXJ is offline   Quick reply to this message
Old 12-03-2012, 11:13 AM   #24 (permalink)
Registered User
 
Join Date: Nov 2011
Member # 203032
Posts: 11
Cool. Thanks. I bought the software and table a year ago, so i bet it is ver3. Yet another of my ID-10-T moments with this thing.
skilawyer is offline   Quick reply to this message
Old 12-18-2012, 09:38 AM   #25 (permalink)
Registered User
 
Join Date: Apr 2007
Member # 89324
Posts: 494
Video coming anytime soon? Or will TM be releasing setup files for the standard tables (in my case a TM 4x4) that has a plate marker and plasma setup?
Conrad_Turbo is offline   Quick reply to this message
 





Quick Reply
Message:
Options

Register Now

In order to be able to post messages on the Pirate4x4.Com : 4x4 and Off-Road Forum forums, you must first register.
Please enter your desired user name, your email address and other required details in the form below.
User Name:
Password
Please enter a password for your user account. Note that passwords are case-sensitive.
Password:
Confirm Password:
Email Address
Please enter a valid email address for yourself.

** A VERIFICATION EMAIL IS SENT TO THIS ADDRESS TO COMPLETE REGISTRATION!! **

Email Address:
Insurance
Please select your insurance company (Optional)

Log-in


Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On



All times are GMT -7. The time now is 03:14 AM.


Powered by vBulletin® Version 3.8.8 Beta 4
Copyright ©2000 - 2020, Jelsoft Enterprises Ltd.
Search Engine Optimization by vBSEO 3.6.0 ©2011, Crawlability, Inc.
User Alert System provided by Advanced User Tagging (Pro) - vBulletin Mods & Addons Copyright © 2020 DragonByte Technologies Ltd.
vBulletin Security provided by vBSecurity v2.2.2 (Pro) - vBulletin Mods & Addons Copyright © 2020 DragonByte Technologies Ltd.