584,814 active members*
5,279 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > MadCAM > madCAM GCode and Tormach PCNC1100 PathPilot not working "out of the box"
Results 1 to 8 of 8
  1. #1
    Join Date
    Feb 2015
    Posts
    57

    Question madCAM GCode and Tormach PCNC1100 PathPilot not working "out of the box"

    With help, I'm comfortable with the toolpaths being generated. However, the G Code that is coming out isn't "machine ready"even though I'm targeting the Tormach PCNC1100 Mach3. I actually have PathPilot which is supposed to use the same G Code commands as Mach3.

    I admit I'm new to this and I very easily could be doing something wrong, but if I am please explain it to me. I'll be glad to learn.

    Here are the issues I'm seeing and wondering if the post processor isn't really 100% working for the Mach 3 TorMach PCNC1100 "out of the box" so to speak:

    First 6 Lines of generated code (untouched by me):
    G00 G49 G40.1 G17 G80 G50 G90 G64
    G20
    (T10_Roughing_FLAT_END_0,25_C30826_30IPM_0.2Depth)
    M6 T10
    M03 S4300
    G01Z3.000


    Line 1: G40.1 is not recognized by PathPilot or GWizardE. What is this supposed to be doing? I don't think it should be in there unless it can be explained. I couldn't find any info on it when I searched for it, just other people getting errors on G40.1.
    Line 1: G50 should be on it's own separate line according to PathPilot.
    Line 6: G01 on this line generates an error in GWizardE saying that the feedrate is not set. If you put G00, the error goes away. When I read up on G00 and G01 I think GWizardE is correct for saying this. A few lines further down and the next G01 in the Z axis has a feedrate specified.

    I had to make the two changes to Line 1 just to be able to run the code on PathPilot. I had already made the change to Line 6 before that point, so I didn't actually test if PathPilot had a problem with Line 6 as it was written.

    Lastly, I have tool offset numbers setup in my tools in madCAM. How come a G49 is being issued? Why are my tool offsets being disabled at this point? (Maybe I'm missing something here or making a mistake myself, so please help me understand if I'm wrong here) I would like to be able to put in my Touch Probe that has a known length and known probe diameter. I'd use this touch probe (tool 99) to set my origin work point 0,0,0. Then I would like to load tool #10 (rougher) which has a known length and diameter and have everything work based on the relative length differences / offsets. For me, Tool 10 also has an entry in the Offset table on row 10. My finishing end mill Tool 11 has an offset entry in Row 11. Since G49 turns off all the offsets, doesn't that ignore that data?

    I'm running my g code as two separate files. Tool 10 Rougher is being run first and Tool 11 Finisher is being run second. I didn't want to have to re-zero when I switch tools. I was thinking that the offsets would take care of that.

    So, it seems like the madCAM default post processor for the Tormach 1100 needs some work out of the box just to generate code that will process (G40.1 removal, G50 on a new line and maybe the G01 on Line 6 being G00?). Then does it need further work to be able to use tool offsets? I could see how that last part might just be personal preference.

    The attached zip file has my Rhino model in inches, the saved workspace, and the 2 different tools that I'm using. T10 has two different files because I have different feed rates set for the different cuts. I've also included a copy of the original output from the post processor. If I make the changes to Line 1, the mill will run up in the air. I'm not confident enough yet to actually try cutting.the work piece yet.

    Any help in understanding what I'm doing wrong, how to correct the post processor and/or understand how to use tool offset numbers properly would be greatly appreciated!

  2. #2
    Join Date
    Mar 2003
    Posts
    35538

    Re: madCAM GCode and Tormach PCNC1100 PathPilot not working "out of the box"

    I had already made the change to Line 6 before that point, so I didn't actually test if PathPilot had a problem with Line 6 as it was written.
    Feedrate is modal, so it remains in effect. It should run, but you won't have any idea how fast it will move. It could run at a default feedratre, or the last feedrate used in a previous program. It looks like a retract, so it should probably be a G00.

    How come a G49 is being issued? Why are my tool offsets being disabled at this point?
    It's common practice to disable tool length offsets when you load your g-code, as if there is a length offset in effect, it may not be the correct offset for the tool you'll be using.
    So you turn off offsets at the start, and then set the offset for the tool before you use it using G43 Hxx.
    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  3. #3
    Join Date
    Feb 2015
    Posts
    57

    Re: madCAM GCode and Tormach PCNC1100 PathPilot not working "out of the box"

    Quote Originally Posted by ger21 View Post
    Feedrate is modal, so it remains in effect. It should run, but you won't have any idea how fast it will move. It could run at a default feedratre, or the last feedrate used in a previous program. It looks like a retract, so it should probably be a G00.
    Thank you for confirming that. I'm glad I'm not doing something wrong by converting it to a G00 to avoid the ambiguity of an undefined feed rate. (Using a default feedrate for an initial retract or using what ever was already set on the mill for feedrate seems sloppy to me. If I'm starting a program, I'd really like it to start the same way every single time.)


    Quote Originally Posted by ger21 View Post
    It's common practice to disable tool length offsets when you load your g-code, as if there is a length offset in effect, it may not be the correct offset for the tool you'll be using.
    So you turn off offsets at the start, and then set the offset for the tool before you use it using G43 Hxx.
    Thank you for explaining this. It definitely addresses part of my question, but I don't think I made the other part of what was confusing me very clear. I entered in all of the offsets into madCAM cutter definitions. Why don't they show up as G43 Hxx commands in the gcode? I only see a command that turns off offsets. I don't see a command that applies any new offsets later on.

    I understand that there are several ways to "begin" from a zero point. I think the way that makes the most sense to me right now (unless someone can tell me the pros of doing it a different/better way) is to use my touch probe (with a known height / offset) to find my 0,0,0 workpiece origin point. Then I do a tool change to my roughing tool (T10) which is called for by my roughing gcode file. It's offset is also known. So I think I want cutter length compensation on from the very beginning, right? (assuming that my zero/origin is already set via touchprobe including its offset?)

    This is more of an understanding how to proceed thing on my part, but if I do want compensation on then do I have to go through the g code and manually add G43 references to tool changes? In this stepped vise jaw example, there is a tool change going from the touch probe to the roughing cutter. Then when I go to the second cutter I'll be in my finishing gcode file and will stay on the finishing cutter the whole time. I figured that it would make sense to run the roughing operation as a single continuous operation and run the finishing step as a single continuous operation with a tool change in between. I just want to make sure that I adjust the gcode properly so I don't mess something up.

    To reiterate: The confusing thing to me is if I put the offset entries into madCAM, how come it doesn't use / apply them automatically? It expects me to handcode the G43 Hxx offsets even though I entered the offset information into the cutter GUI? I wish there was more documentation on madCAM. The help file is a good start, but it really doesn't help you cut your first part.

    Thanks for the reply. It really did help, but I do have a lingering concern.

  4. #4
    Join Date
    Mar 2003
    Posts
    35538

    Re: madCAM GCode and Tormach PCNC1100 PathPilot not working "out of the box"

    Then I do a tool change to my roughing tool (T10) which is called for by my roughing gcode file. It's offset is also known. So I think I want cutter length compensation on from the very beginning, right?
    No. You set the offset for the specific tool, in this case, it would be G43 H10. If the previous program used tool #5, and you left the offset on, then your tool #10 would cut at the wrong depth.

    I've never used MadCAM or PP, so I can't help with the post processor.

    This would appear to be a post processor issue.
    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  5. #5
    Join Date
    Feb 2015
    Posts
    57

    Re: madCAM GCode and Tormach PCNC1100 PathPilot not working "out of the box"

    Quote Originally Posted by ger21 View Post
    No. You set the offset for the specific tool, in this case, it would be G43 H10. If the previous program used tool #5, and you left the offset on, then your tool #10 would cut at the wrong depth.

    I've never used MadCAM or PP, so I can't help with the post processor.

    This would appear to be a post processor issue.
    Again, my question must not have come across properly. I apologize. I wasn't talking about leaving compensation on and then doing nothing about it after that point...I'm trying to understand EXACTLY what I have to do. (capitol letters only for emphasis, not shouting)

    It still seems to me that I would want tool length compensation on *AND* a G43 H10 command to tell it to load the proper offset for that tool change.

    That would be after or instead of the M6 T10 command?

    I understand that you can't comment on madCAM itself. I'm hoping that someone else will chime in because I still want to know why madCAM doesn't use the tool offsets that I put into the cutter definition. That seems like a complete waste of time and a TON of confusion to have fields that are just ignored with no documentation to tell you how/when/why those fields are used. The help file tells me the definition of the field, but it doesn't tell me what I have to do to use the offsets (even if that answer is that I have to go back and put them into the gcode manually...)



    Let's start at the beginning of what I think would happen and make corrections to my understanding based on this:

    Say, I start my gcode script and the very first command is a pause statement telling me to zero my work piece with my touch probe using the offset table for the touch probe.
    So, I zero my work piece and obtain a 0,0,0 that matches my origin from CAD/CAM.
    To do this, I use my touch probe, with it's tool offset loaded.
    I continue my gcode script past the pause statement.
    The "setup" lines are run with tool offset compensation turned on.
    The tool change to T10 is called via the M6 command.
    G43 H10 is called to enable the offset compensation for that new tool based on row 10 in the offset table.


    When the roughing operation is done, I load the finishing file.
    The first command there is a pause to verify that the work piece origin is already zeroed. (Making sure that I am running the finishing operation right after the roughing operation, I shouldn't have to find the origin again. If I shutdown and come back later to run the finishing operation, then I would need to refind the zero with the probe.)
    Either way, I continue the gcode script and it runs with offset compensation turned on.
    Tool change to T11 is called.
    G43 H11 is called to enable the offset compensation for that cutter.
    The rest of the finishing script runs because there are no more tool changes, just different feeds and speed for different operations using the same cutter.

    Do I have to do anything else to utilize offset compensation?

    Don't I have to use offset compensation from the very beginning in order to use my touch probe to find my zero reference? If I

    Am I on the right track? (If I made a mistake, let's correct the mistake without throwing out the whole concept.... I think I want offset compensation ON from the very beginning because I am starting from a known point and I should be able to have a repeatable procedure that I can follow if I understand it.)

    The part that really bugs me is that I put all the tool length and offset information into madCAM. I have no documentation to explain what it is doing with that information and as far as I can tell, madCAM is ignoring the tool offsets. So is it ignoring anything else? Is it ignoring tool lengths? Is it compensating for different cutter lengths since my tool information is all entered into it's cutters? (It bugs me that one field is ignored, so what else is ignored?)

  6. #6
    Join Date
    Apr 2003
    Posts
    1354

    Re: madCAM GCode and Tormach PCNC1100 PathPilot not working "out of the box"

    If you want to use the value from the tool length field when saving a tool you need to add this to your post:

    *TOOL_LENGTH_OFFSET* // Set Yes for using tool length from the saved cutters. (straight out of the help file)

    I'm not familiar with your machine or controller, but I'll give you a general overview of how it's typically done.

    Before you run your g-code, you need to know what tools you will need. Place those tools in the tool turret, then pick up the length of each tool. Enter that length in your tool table (I'm assuming your machine has one for length and diameter). Now the length offset is tied to a tool number. Then run the code. By having G43Hxx in your code, you are telling the controller to use that pre-set length with the tool.

    You don't need to enter a value in madCAM. If you do want to use that feature, then you need to add what I copied and pasted above to your post.

    Hope this helps,

    Dan
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  7. #7
    Join Date
    Feb 2015
    Posts
    57
    Quote Originally Posted by Dan B View Post
    If you want to use the value from the tool length field when saving a tool you need to add this to your post:

    *TOOL_LENGTH_OFFSET* // Set Yes for using tool length from the saved cutters. (straight out of the help file)

    I'm not familiar with your machine or controller, but I'll give you a general overview of how it's typically done.

    Before you run your g-code, you need to know what tools you will need. Place those tools in the tool turret, then pick up the length of each tool. Enter that length in your tool table (I'm assuming your machine has one for length and diameter). Now the length offset is tied to a tool number. Then run the code. By having G43Hxx in your code, you are telling the controller to use that pre-set length with the tool.

    You don't need to enter a value in madCAM. If you do want to use that feature, then you need to add what I copied and pasted above to your post.

    Hope this helps,

    Dan
    That helps a lot. I wasn't sure that it was just the g43h## command. Thank you for confirming that would do it along with how to add it to post. I didn't see that in the help file. What section was it in? I'll look and see what else I missed.

    I already have offset 10 and 11 defined in the mill controller. Length and diameter areinforced set.

    Combined that with a couple other fixes and it looks like I have code that should run.

  8. #8
    Join Date
    Apr 2003
    Posts
    1354

    Re: madCAM GCode and Tormach PCNC1100 PathPilot not working "out of the box"

    It was in the post-processor section. Everything in the current release of madCAM works. Is it perfect? Nope, not yet. But we are working on it. Often when something doesn't seem right, like in this case, it's just a matter of understanding it better. For example, not every function is enabled in default post-processors. That means some features may need to be "turned on" by adding the appropriate sections to the post. Anyone can do it. It's not difficult at all.

    Dan
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

Similar Threads

  1. How to "Drill" a 1/2-20 thread hole 1" deep on a Tormach in Ti-6Al4V
    By ChrisPhoenix in forum Material Machining Solutions
    Replies: 10
    Last Post: 07-18-2015, 01:05 AM
  2. Replies: 4
    Last Post: 05-15-2015, 06:00 PM
  3. Replies: 0
    Last Post: 12-11-2014, 06:27 PM
  4. Anyone Using A Tormach 17mm "Modular" Endmill with the "Medium" Adaptor?
    By SCzEngrgGroup in forum Tormach Personal CNC Mill
    Replies: 15
    Last Post: 11-03-2014, 09:17 PM
  5. X Axis "Goes Off Pattern", "Awry", "Skewed", "Travels"
    By DaDaDaddio in forum Laser Engraving / Cutting Machine General Topics
    Replies: 1
    Last Post: 05-06-2013, 09:59 AM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •