Different feeds and speeds for same cutter in group postprocessing.


Results 1 to 17 of 17

Thread: Different feeds and speeds for same cutter in group postprocessing.

  1. #1
    Member AvB's Avatar
    Join Date
    Sep 2012
    Location
    Australia
    Posts
    62
    Downloads
    0
    Uploads
    0

    Default Different feeds and speeds for same cutter in group postprocessing.

    I've been using Rhino and Madcam for about 18 months now and have great results generally, but of course there are always new things to work out.

    I am a bit confused about how the cutter settings work with post-processing.

    Let’s say I want to use the same cutter for a number of different toolpaths doing different functions, and then post process them all together in one file.

    Initially I choose the cutter settings (feed, speed, tolerance etc) when creating the first toolpath. Then I make the next toolpath using the same cutter, but I want to change the settings … for example I the first path may be to rough out one section with a fast speed and easy tolerance, but then the next path might be fine finish with slower speed and fine tolerance. But when I post process the toolpaths as one file, it will only assign one feed/ speed setting to all of the toolpaths, and it’s always the SAVED settings. It doesn’t use the settings that you change and “OK”, unless you save them as the new cutter file. But then it will apply those settings to all toolpaths that you are post processing together. I can’t work out how to get different feeds and speeds to be included in one file.

    Is that how it’s meant to be?

    Similar Threads:


  2. #2
    Member
    Join Date
    Mar 2010
    Location
    Canada
    Posts
    66
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    As far as I understand, the design of the madcam tool system implies that you need to save each feed & speed setting under a new tool name.

    I have been doing this by giving long names to each tool setting which include descriptions such as wood roughing, aluminum finishing etc.



  3. #3
    Member AvB's Avatar
    Join Date
    Sep 2012
    Location
    Australia
    Posts
    62
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Thanks. OK, so I guess you can still postprocess them together if they are the same cutter size, and just ignore the M6's?



  4. #4
    Community Moderator
    Join Date
    Mar 2004
    Location
    Sweden
    Posts
    1661
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    From my point of view, that's wrong way to do it.
    A cutter should run with optimal speed and RPM for best result, when you lower the speed or RPM to get better result in another operation you are in either one of them running the cutter under circumstances it wasn't made for. I know what type of machine you have and running cutters with slow feed will make then "rub" away material instead of cutting. If I were you I would keep the speed/RPM and run the fine path with more (narrow) lines and less depth.
    Consider changing the way you work, that's my recommendation.



  5. #5
    Member AvB's Avatar
    Join Date
    Sep 2012
    Location
    Australia
    Posts
    62
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Thanks very much Sven. OK, I understand what you're saying. I almost exclusively cut the moulds in Corian (or similar solid benchtop) acrylic and it is very tolerant of feeds and speeds. I was thinking that with some 3D cuts I have to cut the feed rate down due to the amount of movement, avoiding CV rounding while keeping the machine movement smooth - and slow the cutter accordingly to keep the chip load correct. Whereas for example 2D profiling can be run at higher feed rates and cutter speeds. I thought I should try to run these different types of toolpaths consecutively if they use the same cutter. But I hear you. I don't have the depth of experience and there's a lot to learn.



  6. #6
    Member
    Join Date
    Mar 2010
    Location
    Canada
    Posts
    66
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Quote Originally Posted by AvB View Post
    Thanks. OK, so I guess you can still postprocess them together if they are the same cutter size, and just ignore the M6's?
    You should be able to keep the same tool number for the same cutter even when saving it to your library with different speeds & feeds. That should take care of any unnecessary tool changes.



  7. #7
    Member AvB's Avatar
    Join Date
    Sep 2012
    Location
    Australia
    Posts
    62
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Ah, that's a great tip, thanks!



  8. #8
    Community Moderator
    Join Date
    Mar 2004
    Location
    Sweden
    Posts
    1661
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Yes, you can have many tools with the same settings as long as the name is unique. I do that too keep the settings for different materials. But still, you're running the same cutter in the same material...



  9. #9
    Member
    Join Date
    Mar 2010
    Location
    Canada
    Posts
    66
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Reviving this thread because I'm running into a related problem:

    I'm finding that madCAM is not generating new S commands when the tool number is staying the same but the spindle speed is changing for a new cutting path.

    Everything is working correctly when the tool number changes: correct speeds & feedrates, but when the same tool number is used then the new feed rate is used but the speed rate is being ignored in the g-code.

    Any tips on how to fix this?

    Leo



  10. #10
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Do you have two identical tools in your library, each representing a different speed? If not, how are you changing the speed?

    Dan

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


  11. #11
    Member
    Join Date
    Mar 2010
    Location
    Canada
    Posts
    66
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Hi Dan,
    Yes I've got two identical tools in my library, each with a different spindle speed and feed rate.



    The toolpaths are all being generated correctly, but in the g-code file the speed and feedrate changes are being ignored for the second tool setting. The first and third tools are showing up correctly in the g-code.

    Could this be caused by an incorrect setting in my post processor file? I'm just using the Mach3-inches post processor file.


    Edit: Ok so I've tried the same toolpaths with a few different post processor files and the results are the same: all speed and feed settings for the second tool are being ignored.

    I can understand that the machine needs to ignore the tool change because it's the same tool number, but how to I get it to accept the new speed and feed rates?

    I suspect I need to learn how to understand and modify or write my own post processor files. I've looked at the help file in madCAM regarding post processors but it looks pretty daunting.

    Attached Thumbnails Attached Thumbnails Different feeds and speeds for same cutter in group postprocessing.-madcam-feedrate-speed-problem-jpg  


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

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Please attach the post you are using. I just test a Doosan post I have and I get the speed change for an identical tool. I suspect it might have to do with where your speed variable is placed in the post. For example, here is mine:

    *FIRST_MOVE*
    N"lnbr" G00G90"fixture_offset""x""y"S"speed"M3
    N"lnbr" G43H"toolnr"D"toolnr""z""coolant_on"
    N"lnbr" M24
    N"lnbr" G00"cutter_comp""x""y"
    N"lnbr" G00"z"
    *END_SECTION*

    Sorry, I don't have the default posts for madCAM. I always write my own.

    Thanks,

    Dan

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


  13. #13
    Member
    Join Date
    Mar 2010
    Location
    Canada
    Posts
    66
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Hi Dan,
    Thanks for your reply and I've attached one of the stock madCAM post processor files I've tried most often.

    I'm searching for resources that can help me learn how to write my own post processor files. If there were any particular resources or tutorials which helped you learn this skill I'd love to hear their names.

    Attached Files Attached Files


  14. #14
    Member
    Join Date
    Mar 2010
    Location
    Canada
    Posts
    66
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Ok so after some experimenting things are making a tiny bit more sense.

    First I tried adding a *FIRST_MOVE* section with the M03 S"speed" variable in it. That caused some redundant speed settings in the G-code output, so I removed the "speed" variable from the *TOOL_CHANGE* section and that has cleaned things up somewhat.

    Except that there are now there are speed commands for every new toolpath regardless of whether I've changed madCAM tool assignments.

    This should work perfectly fine on my machine, however I'm still not getting how to tweak the post processor to only assign new speeds and feeds only when I've assigned a new madCAM tool, even if that tool has the same tool number.



    At least now my eyes have been opened to what kind of stuff post processor files actually do. I can see that I should be able to exert very fine control over my machine behavior if I can understand more of the post processor commands.



  15. #15
    Member
    Join Date
    Mar 2010
    Location
    Canada
    Posts
    66
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Ah this looks like what I'm looking for:

    *TOOLPATH_CHANGE*
    M03 S"speed"
    *END_SECTION*

    This is putting the speed in at the beginning of each path, so I've taken the "speed" variable out of the *TOOL_CHANGE* command and put it here instead and that solves the missing speeds problem. It's still putting more speeds than is strictly necessary in situations where a new path starts with the same tool and speed, but that does no harm I think.

    So as far as I can see madCAM will ignore the "TOOL_CHANGE* command whenever the tool number hasn't changed from the previous tool number. Can anyone confirm if this is correct?


    Definitely getting more comfortable with the post processor editing workflow now. I can see that writing your own is quite practical once you're comfortable with the meaning of the post processor commands and variables.



  16. #16
    Member Dan B's Avatar
    Join Date
    Apr 2003
    Location
    Ontario
    Posts
    1354
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Yes, you are correct. If the same tool number is used on the next path the *TOOLPATH_CHANGE* section is used, not the "TOOL_CHANGE* section.

    Also, I've never seen any adverse effects of calling the spindle speed for a tool, even if it's the same as what's already there.

    As for post writing guidance, it's all there in the help file. I've never run across any other documentation for madCAM posts. It's actually very simple once it clicks in, as I think you are discovering.

    Dan

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


  17. #17
    Member
    Join Date
    Mar 2010
    Location
    Canada
    Posts
    66
    Downloads
    0
    Uploads
    0

    Default Re: Different feeds and speeds for same cutter in group postprocessing.

    Thanks very much for your confirmation and help Dan.

    I think it's really coming together for me now as far as understanding how the post processing works.


    I seem to have come across a very minor glitch: the variable "documentname" is not returning anything. It would be nice to reference the Rhino file which was used to generate the g-code.

    Edit: Whoops, didn't know there has already been a thread created on this.

    Leo

    Last edited by Corvus; 05-22-2017 at 08:03 PM. Reason: Thread already exists.


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

Different feeds and speeds for same cutter in group postprocessing.

Different feeds and speeds for same cutter in group postprocessing.