Post Processor for WinCNC


Page 1 of 2 12 LastLast
Results 1 to 20 of 25

Thread: Post Processor for WinCNC

  1. #1
    Registered
    Join Date
    Feb 2013
    Location
    US
    Posts
    19
    Downloads
    0
    Uploads
    0

    Question Post Processor for WinCNC

    Hey everyone,

    I'm about half way through my trial of madCAM right now and am getting the hang of it but I have not yet been able to post. I have a CAMaster Stinger which is controlled by wincnc.

    Does anyone have the right post processor file for me, or could you point me in the right direction?

    Also, I've noticed that when I try to open files from the madcam browse box the window explorer seems to show folders only. It doesn't show files, for example, text files in the folder I'm in, even though it's looking for txt files.

    Thanks for the help!

    Similar Threads:


  2. #2
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    If you post an example of code that you would like to see output from madCAM's post, I can probably help you.

    Dan

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


  3. #3
    Registered
    Join Date
    Feb 2013
    Location
    US
    Posts
    19
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Awesome, thanks! edit: I'm not sure if you'll need to see other codes that wincnc uses or not, I just grabbed a random .nc file I had laying around.

    G90
    M3
    S18000
    G0 Z1.9842
    G0 X0.6553 Y0.7888
    G1 X0.6553 Y0.7888 Z1.0250 F30.
    G1 X0.6553 Y0.7888 Z1.0244 F70.
    G1 X0.6553 Y0.7887 Z1.0078

    //Redacted for brevity

    G1 X0.6553 Y2.7888 Z0.3000
    G1 X0.6554 Y2.7888 Z0.3000
    G1 X0.6553 Y2.7888 Z0.3000
    G0 Z1.9842
    G0 X0.6553 Y2.7888
    M5
    G53 Z
    X0Y0




  4. #4
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Does your machine have a tool changer?

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


  5. #5
    Registered
    Join Date
    Feb 2013
    Location
    US
    Posts
    19
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Nope...

    lol.



  6. #6
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Try this:

    https://onedrive.live.com/redir?resi...int=file%2ctxt

    I didn't add support for coolant on/off (although everything is in place to add that if you wish). I also didn't add fixture offsets (G54, G55 etc.) Let me know if you need that.

    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
    Registered
    Join Date
    Feb 2013
    Location
    US
    Posts
    19
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Thank you so much! I am on a different computer now but I'll try it out ASAP. I haven't used fixture offsets yet, but may in the future. However, I always figured it'd be just as easy or easier to just copy and paste the model and toolpaths in Rhino, so who knows, I may never use those codes.

    Thanks again, I very much appreciate you taking the time to help out.



  8. #8
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    No problem. I hope your trial of madCAM goes well.


    Dan

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


  9. #9
    Member
    Join Date
    Mar 2008
    Location
    US
    Posts
    1762
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    JMB...
    As an FYI the code that you have posted will probably work, but is not in line with current WinCNC recommendations. If you posted that using a Vectric product, select and download one of the current CAMaster postP's from the Owners section of the CAMHeads forum.

    Gary Campbell GCnC Control
    Servo Control & ATC Retrofits


  10. #10
    Registered
    Join Date
    Feb 2013
    Location
    US
    Posts
    19
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Quote Originally Posted by islaww View Post
    JMB...
    As an FYI the code that you have posted will probably work, but is not in line with current WinCNC recommendations. If you posted that using a Vectric product, select and download one of the current CAMaster postP's from the Owners section of the CAMHeads forum.
    Hmm, that's interesting. I was using rhinocam before and it already had a wincnc postp in it. It had to be edited slightly by taking out a T4 command (iirc) at the begging, but besides that it has worked well.

    Thanks Gary



  11. #11
    Registered
    Join Date
    Feb 2013
    Location
    US
    Posts
    19
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Hey Dan, just posted with the new postp for the first time. The code is coming out with N and the line number, but not G0 or G1 like my old code did. Is this by design? Also, any idea why I can't see files in the explorer browser? I have to manually type in the filename and then hit enter.



  12. #12
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Sorry, I made the assumption that the line numbers would work for you. I will remove them. Also, I failed to notice that the G1 was non-modal. Here is a revised version. Let me know if this one works.

    https://onedrive.live.com/redir?resi...int=file%2ctxt

    Generally there is a "safety line" in the beginning of the g-code. I don't want to make any more assumptions, but maybe you would like to manually edit the code and try these:

    G17 ~working in the XY plane
    G40 ~cutter comp cancel
    G80 ~fixed cycle cancel

    If you want I can add those to the G90 right at the beginning.

    With regard to fixture offsets, the advantage is that you can create separate programs, mount the stock to your machine table anywhere you want, pick up each and assign an offset. Doing it this way as opposed to positioning in Rhino means that your set-up is a lot easier. If you splice your G-code together you can concatenate your paths and potentially run lights out.

    I'm not sure I understand your question about Windows Explorer. Are you referring to the code, with the .nc extension? Could you attach a screen capture of the issue?

    Thanks,

    Dan

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


  13. #13
    Registered
    Join Date
    Feb 2013
    Location
    US
    Posts
    19
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    I didn't mean to say that they didn't work! I was just noting differences, the other being that the G commands were not before the coordinates. Is that what was off about my code before? No need to have all those G1s output, the xy coordinate itself is sufficient? Sorry, I haven't studied gcode much. I pretty much only ever type g92, m3 or m5, but now that I think of it, it makes sense that the G1 is unnecessary. I haven't ran any of the code on the machine yet, but I'm guessing it will work just fine.

    When I press the open or browse button to select the post processor file (or elsewhere when madcam tries to find a file) the file explorer window that pops up does not show any files, only folders. I can fetch the file by typing the name into the box, but I can't visually see it to select it.

    In my image, there are text files in the folder I'm viewing, I just can't see them.

    Post Processor for WinCNC-screen-jpg



  14. #14
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Whether or not you need the G1 on every line will depend on your controller. All Fanuc based controllers that I've worked with are modal. That means that most (but not all) functions (like G1, G0 etc.) are remembered by the controller until another command bumps it out of the memory. Not sure if that's the best explanation, but that's basically how it works. So if a G1 appears on a line, all of the following lines have G1 applied until something else like a G0, G2, G3 etc. takes over. If the machine is non-modal, you need a command on every line. The good news is that having G1 on every line will work for both scenarios.

    As for your explorer issue, you are in the place where you select your default machine template. It's looking for a folder. I'm pretty sure that whatever you are trying to do, you are in the wrong spot.

    Dan

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


  15. #15
    Member
    Join Date
    Mar 2008
    Location
    US
    Posts
    1762
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Guys...
    Here is the currently supported header for WinCNC control. For machines without ATC or a manual multiple toolchange system, remove the "T" calls. Ignore extraneous info.

    [VECTRIC CNC OUTPUT FOR CAMASTER TOOLCHANGE ]
    [MACHINES WITH WINCNC CONTROL ONLY]

    [FILENAME: Training Cabinet Parts]
    [10:50 AM, Saturday May 09 2015]

    [MATERIAL size: 48.000" x 96.000" x 0.750"]
    [Z Zero Position: Table Surface]

    [TOOL LIST]
    [1 = End Mill (0.375 inch)]
    [2 = End Mill (0.25 inch)]
    [3 = Drill (5mm)]
    [4 = 375 Compression]

    G90 [ABSOLUTE MODE]

    M5 [SPINDLE OFF]
    G53 Z0 [LIFT Z TO TOP]

    T1 [ GET TOOL NUMBER 1 ]
    [End Mill (0.375 inch)]

    S13500 [ SET SPINDLE SPEED RPM ]
    M3 [SPINDLE ON]

    G53 Z0 [LIFT Z TO TOP]

    [TOOLPATH NAME: Pocket Dados]
    F400 XY [SET FEEDRATE FOR X AND Y]
    F250 Z [SET FEEDRATE FOR Z]

    G0 X-0.062500 Y4.187500
    G0 Z2.000
    G1 X-0.062500 Y4.187500 Z0.500000
    G1 X23.562500 Y4.187500 Z0.500000
    G1 X23.562500 Y4.562500 Z0.500000
    G1 X-0.062500 Y4.562500 Z0.500000
    G1 X-0.062500 Y4.187500 Z0.500000
    G0 X-0.062500 Y4.187500 Z0.950000

    Gary Campbell GCnC Control
    Servo Control & ATC Retrofits


  16. #16
    Registered
    Join Date
    Feb 2013
    Location
    US
    Posts
    19
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Thanks, Gary. I'm not sure how, but I'm assuming that this that information is used to create custom post processors for different CAM packages?

    Dan, the file explorer was looking for the post processor file. As you can see, it says "File name:" before the box, and then shows to the right that it is looking for .txt files. It shows no files, but when I begin typing the file name it knows that its there and allows me to click it. I accessed this explorer window from that machine tab and then clicking the open button to select my post processor. It has the same peculiarity elsewhere when trying to open files.

    I haven't been taken a break from learning madCAM because I installed the trial on my CNC pc as well and it was crashing rhino, iirc it was when I went to load the post processor. Perhaps I should start a different thread for other questions related to madCAM but I was also having issues editing the saved toolpath that I had worked on with my laptop.. perhaps because the tool library was on my laptop? but there was no easy way to just reselect the tool from the CNC pc library. Also, when I go to select tool rather than madCAM remembering where my tool library is, I have to navigate to the folder every time I open the tool dialog. Is this normal? One other question comes to mind (though I'm sure I'll remember more), I watched a video on scripting the MC commands with their settings, but I noticed when I ran a MC operation such as creating a profiling toolpath, it would show the MC_Profiling (or whatever the command is) but it did not show the settings to copy and paste for scripting.

    Lots of questions, I know, but I really want to become proficient enough in the software to feel comfortable buying it. I feel like it has a lot of potential, but so far it has seemed a bit buggy to me. Really hoping to become proficient in it, as the educational license is in my price range and I also think the ability to script the commands could make the whole process very efficient.

    Thanks again for the help!



  17. #17
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    You are going about this wrong. In the options you set up a machine template. When the template is done correctly all you do is pick your machine and the tool libraries and posts are synchronized automatically. Here is how to do it. First, go to the options and pick the machine tab (the place you were at). Pick the machine description that suits your machine:

    Post Processor for WinCNC-figure-1-png

    Now just to the left, rename the machine to something more descriptive:

    Post Processor for WinCNC-figure-2-png

    Now you go to the machine library and browse to your machine folder. It's going to be in C:\ProgramData\5XCNC\madCAM\5.0\Machines. Don't expect to find a file here at this time. You are just defining where this template will be saved. Now go to the Post Processor button and select the post that you want to associate with this template. Now do the same thing for the tool library. Note that it's possible to have a separate tool library for each machine, and differing materials. Once you've made that selection, save the template using the save button at the top, then pick the new machine out of the list on the bottom right:

    Post Processor for WinCNC-figure-3-png

    Now pick OK to close the Options window. Now reopen it and go to the General tab. Go to the default machine window and pick the arrow to see your list. Pick your new machine out of the list. If you only have one machine you probably will never need to do this again. In our case we have many, so we often come to the general tab to switch to the appropriate machine.

    Post Processor for WinCNC-figure-4-png

    Now when it's time to post your code, just go to the post processor icon and stay out of the options.

    Hope this helps,

    Dan

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


  18. #18
    Registered
    Join Date
    Feb 2013
    Location
    US
    Posts
    19
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Dan, thanks so much, that helped a lot!

    My c:/programdata folder was hidden, and after unhiding I was able to save my cutters and the folder was loaded automatically rather than having to navigate to it every time. I am still not able to see files when browsing, for example, to select the post processor file. This is true for both my laptop and CNC pc. This isn't really a big deal at all, I just thought it was peculiar and that yall would want to know.

    On my CNC pc I am unable to simulate, presumably because of the weak onboard gfx card.

    I finally posted and ran some g-code and everything worked nicely!

    A few questions:

    -If I want different operations with the same tool done at different feeds, is the way to do this to make several cutters and vary the feed?

    -Is there a way to recalculate all tool paths after editing a curve or model?

    -If I have an operation but I want to either change or add curves, is there any easy way to do this without remaking the path from scratch?

    -It seems like the process will be streamlined when I figure out the scripting. I watched a video on youtube on scripting madCAM, but when I run a madCAM command all I see in the command line is the command itself, no settings to copy and paste.

    Thanks again!!!
    Justin



  19. #19
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Hi Justin,

    Are you saying that you don't see your post here:

    Post Processor for WinCNC-post-jpg

    A few questions:

    -If I want different operations with the same tool done at different feeds, is the way to do this to make several cutters and vary the feed?

    Yes. I created libraries for various materials and for numerous machines. You sync it all like I explained a few posts back. Then when you have a project, say steel for your Fadal, you pick that template on the first page of the options and your tool library will be the default.

    -Is there a way to recalculate all tool paths after editing a curve or model?

    Currently only one at a time. I believe there are some changes coming with regard to recalculating, so we'll just have to wait and see. However, you can save out templates and just import them. I believe there is a video on YouTube illustrating that. It works well, we do it all the time.

    -If I have an operation but I want to either change or add curves, is there any easy way to do this without remaking the path from scratch?

    Making paths is so quick that I've never considered that, but it's probably something that could be discussed. I usually would just use my middle mouse button, call up the command again and pick my newly modified curve.

    -It seems like the process will be streamlined when I figure out the scripting. I watched a video on youtube on scripting madCAM, but when I run a madCAM command all I see in the command line is the command itself, no settings to copy and paste.

    Scripting in madCAM is on my to-do list. I've done extensive scripting with both VBscript and Python for Rhino, so I'm eager to see what I can do with madCAM. It's just a matter of finding time.

    Hope there's something helpful here.

    Dan

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


  20. #20
    Member
    Join Date
    Apr 2014
    Posts
    15
    Downloads
    0
    Uploads
    0

    Default Re: Post Processor for WinCNC

    Quote Originally Posted by Dan B View Post
    If you post an example of code that you would like to see output from madCAM's post, I can probably help you.

    Dan

    Hi Dan,
    Would you possibly be able to help me with a WINCNC post for a ShopSabre machine that I would like to run AlphaCAM on? They make it extremely expensive and difficult to acquire, though it's great software and I've been using it on a 5X10 Flexicam machine for the last 14 years.

    Thanks for any consideration,
    Anton



Page 1 of 2 12 LastLast

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
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Post Processor for WinCNC

Post Processor for WinCNC