Loading ...
Sorry, an error occurred while loading the content.

RhinoCAM 2012 issue (not running on Mach3)

Expand Messages
  • steven_dantonio
    Hi, I m making this inquiry on t unrelated forums at the same time. Also, I don t thing I can attach files to a post in a yahoo forum (at least I haven t
    Message 1 of 9 , Mar 23, 2013
    • 0 Attachment
      Hi,

      I'm making this inquiry on t unrelated forums at the same time. Also, I don't thing I can attach files to a post in a yahoo forum (at least I haven't figured out how to o it yet). I can send anyone the tow posts and the rhino file is anyone wants to look at them.

      I am a long time user of RhinoCAM 1.0 on Rhino (3 and 4) without any issues

      Recently I upgraded to Rhino 5 and finally installed RhinoCAM 2012 (lucky for me I kept the old Rhino 4 on the system).

      The steps I have taken and the issue is this:

      1. I started Rhino5 (with RhinoCAM 2012) and made sure all the units were set to inches
      2. I drew a test part (a circle and a square)
      3. I set up 2 simple profiling operations and ran a simulation in RhinoCAM which worked fine (shown below as simulation)
      4. I posted the results using Mach3-inch in RhinoCAM 2012 and got the file (g-code available if you want to see it)
      5. I loaded it into Mach3, started up the system and tried a test cut, nothing moved.
      6. I took the same part file and brought it up in Rhino4 (with RhinoCAM 1.0) and generated the following output (g-code available if you want to see it)
      7 Set up the same test cut on the CNC and it worked perfectly as expected from looking at the g-code.

      In both cases I'm running RhinoCAM 4 and 5 on a Pentium 4, g GHz machine running WinXP SP3 (don't know if this is significant)

      The only response I got so far is (quoted below):

      "The only significant difference in the two G-code files is that the Rhino4 version is all done with G01 (directional commands at a feedrate) while the other uses G03 commands (move in an arc defined by I and J). This is a little trickier for Mach3 to interpret; make sure your postprocessor is in "absolute" mode for this sort of thing. You can also tell RhinoCAM to break down arcs into segments, as it was doing previously."

      When responding please consider me to be g-code illiterate, so, is this issue with the G03 commands something that can be solved at the mach 3 end or is it something that needs to be solved at the RhinoCAM end of things?

      Thank you,
      Steven
    • quadconversions
      Hi Steven, I m interested in this one too. I m g-code illiterate as well, but I understand that I and J commands make smooth curves making a machine faster and
      Message 2 of 9 , Mar 24, 2013
      • 0 Attachment
        Hi Steven,

        I'm interested in this one too. I'm g-code illiterate as well, but I
        understand that I and J commands make smooth curves making a machine faster and
        smoother. That's worth upgrading RhinoCam.

        You seem to have found Mach 3 can't handle this... is this right guys?
        I'm guessing Mach 4 will...?

        Regards Dave K


        In a message dated 24/03/2013 04:12:23 GMT Standard Time,
        sdantonio93@... writes:

        Hi,

        I'm making this inquiry on t unrelated forums at the same time. Also, I
        don't thing I can attach files to a post in a yahoo forum (at least I
        haven't figured out how to o it yet). I can send anyone the tow posts and the
        rhino file is anyone wants to look at them.

        I am a long time user of RhinoCAM 1.0 on Rhino (3 and 4) without any issues

        Recently I upgraded to Rhino 5 and finally installed RhinoCAM 2012 (lucky
        for me I kept the old Rhino 4 on the system).

        The steps I have taken and the issue is this:

        1. I started Rhino5 (with RhinoCAM 2012) and made sure all the units were
        set to inches
        2. I drew a test part (a circle and a square)
        3. I set up 2 simple profiling operations and ran a simulation in RhinoCAM
        which worked fine (shown below as simulation)
        4. I posted the results using Mach3-inch in RhinoCAM 2012 and got the file
        (g-code available if you want to see it)
        5. I loaded it into Mach3, started up the system and tried a test cut,
        nothing moved.

        6. I took the same part file and brought it up in Rhino4 (with RhinoCAM
        1.0) and generated the following output (g-code available if you want to see
        it)
        7 Set up the same test cut on the CNC and it worked perfectly as expected
        from looking at the g-code.

        In both cases I'm running RhinoCAM 4 and 5 on a Pentium 4, g GHz machine
        running WinXP SP3 (don't know if this is significant)

        The only response I got so far is (quoted below):

        "The only significant difference in the two G-code files is that the
        Rhino4 version is all done with G01 (directional commands at a feedrate) while
        the other uses G03 commands (move in an arc defined by I and J). This is a
        little trickier for Mach3 to interpret; make sure your postprocessor is in
        "absolute" mode for this sort of thing. You can also tell RhinoCAM to break
        down arcs into segments, as it was doing previously."

        When responding please consider me to be g-code illiterate, so, is this
        issue with the G03 commands something that can be solved at the mach 3 end or
        is it something that needs to be solved at the RhinoCAM end of things?

        Thank you,
        Steven





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

        www.machsupport.com - Web site AccessYahoo! Groups Links







        [Non-text portions of this message have been removed]
      • ionsignal
        Steven, I have dealt with postprocessor issues in Mastercam, but most likely same way to resolve in RhinoCam. The Post processor is a file that tells the
        Message 3 of 9 , Mar 24, 2013
        • 0 Attachment
          Steven,

          I have dealt with postprocessor issues in Mastercam, but most likely same way to resolve in RhinoCam.

          The Post processor is a file that tells the software how to output the moves in Gcode format. Each machine has its own way it likes to see the gcode to run. There are sections of the post file that sets up the beginning of the gcode file and sections that setup the motion parts and sections that setup the ending of the gcode file. And there is the 'main' section that sets up the actual motion parts of the gcode file. The begging and ending parts can be the most important parts for they are the parts that set the machine tool into safe states for the start of motion.

          I would take a gcode file from your previous version and compare line by line with one from the new version and note the differences.

          inspect the post file to figure out, it can seem cryptic because of the C type of format, and see what is generating the line of gcode you want to change.

          Or better still, get a post from another user that has been altered for Mach, but you may want to learn how to edit a post yourself.

          As far as circle cutting, there are a few ways to tell a machine to cut an arc and Mach likes only one of those ways, I think. Look at the manual or on of the posted gcodes from when it worked.

          Hope this helps,

          Mark

          --- In mach1mach2cnc@yahoogroups.com, "steven_dantonio" <sdantonio93@...> wrote:
          >
          > Hi,
          >
          > I'm making this inquiry on t unrelated forums at the same time. Also, I don't thing I can attach files to a post in a yahoo forum (at least I haven't figured out how to o it yet). I can send anyone the tow posts and the rhino file is anyone wants to look at them.
          >
          > I am a long time user of RhinoCAM 1.0 on Rhino (3 and 4) without any issues
          >
          > Recently I upgraded to Rhino 5 and finally installed RhinoCAM 2012 (lucky for me I kept the old Rhino 4 on the system).
          >
          > The steps I have taken and the issue is this:
          >
          > 1. I started Rhino5 (with RhinoCAM 2012) and made sure all the units were set to inches
          > 2. I drew a test part (a circle and a square)
          > 3. I set up 2 simple profiling operations and ran a simulation in RhinoCAM which worked fine (shown below as simulation)
          > 4. I posted the results using Mach3-inch in RhinoCAM 2012 and got the file (g-code available if you want to see it)
          > 5. I loaded it into Mach3, started up the system and tried a test cut, nothing moved.
          > 6. I took the same part file and brought it up in Rhino4 (with RhinoCAM 1.0) and generated the following output (g-code available if you want to see it)
          > 7 Set up the same test cut on the CNC and it worked perfectly as expected from looking at the g-code.
          >
          > In both cases I'm running RhinoCAM 4 and 5 on a Pentium 4, g GHz machine running WinXP SP3 (don't know if this is significant)
          >
          > The only response I got so far is (quoted below):
          >
          > "The only significant difference in the two G-code files is that the Rhino4 version is all done with G01 (directional commands at a feedrate) while the other uses G03 commands (move in an arc defined by I and J). This is a little trickier for Mach3 to interpret; make sure your postprocessor is in "absolute" mode for this sort of thing. You can also tell RhinoCAM to break down arcs into segments, as it was doing previously."
          >
          > When responding please consider me to be g-code illiterate, so, is this issue with the G03 commands something that can be solved at the mach 3 end or is it something that needs to be solved at the RhinoCAM end of things?
          >
          > Thank you,
          > Steven
          >
        • steven_dantonio
          Hi Mark, I started to do a line by line comparison and then gave up because the RhinoCAM 2012 file is about 20 lines long and the RhinoCAM 1.0 file is about
          Message 4 of 9 , Mar 24, 2013
          • 0 Attachment
            Hi Mark,

            I started to do a line by line comparison and then gave up because the RhinoCAM 2012 file is about 20 lines long and the RhinoCAM 1.0 file is about 100 lines long or longer. It looks like the RhinoCAM 1 file approximates the arcs as a series of short straight lines (each move being a separate line of g-code.

            This is the RhinoCAM 1.0 header

            G17 G21 G40 G54 G64 G90
            (2 1/2 Axis Profiling)
            T1 M6
            (0.25)
            G00 Z3.1750
            X3.1753 Y3.1753
            G01 Z-1.5875 F1199.999988
            X57.5650 F1199.999988
            X59.1673 Y5.5150
            X60.5948 Y7.9653
            X61.8400 Y10.5131


            this is the entire RhinoCAM 2012 file

            G00 G49 G40.1 G17 G80 G50 G90
            G20
            (2 1/2 Axis Profiling)
            M6 T1
            M03 S12223
            G00 Z0.3750
            X1.1250 Y4.0000
            G01 Z0.0625 F100.0
            X1.8750
            Y5.5000
            X1.1250
            Y4.0000
            Z0.0000
            X1.8750
            Y5.5000
            X1.1250
            Y4.0000
            G00 Z0.3750
            X0.1250 Y0.1250
            G01 Z0.0625 F100.0
            X2.2663
            G17
            G03X0.1250Y2.2663I-1.2308J0.9105
            G01 Y0.1250
            Z0.0000
            X2.2663
            G03X0.1250Y2.2663I-1.2308J0.9105
            G01 Y0.1250
            G00 Z0.3750
            M5 M9
            M30


            The ends of both codes look pretty much the same.

            On startup with the RhinoCAM 2012 file it appears that Mach3 immediately jumps to this line

            G03X0.1250Y2.2663I-1.2308J0.9105

            and them stops dead.

            One thing I did try is to take the post from 1.0. drop it into the post folder in 2012 and call that up as the post file. But I got results identical to the regular 2012 mack3-inch post. So it doesn't seem to be in the post file itself, but in how 2012 is controlling that file. It's probably just some dumb toggle switch or radio button somewhere. I just need someone to point out which one it is.

            Steven

            --- In mach1mach2cnc@yahoogroups.com, "ionsignal" <mhager@...> wrote:
            >
            > Steven,
            >
            > I have dealt with postprocessor issues in Mastercam, but most likely same way to resolve in RhinoCam.
            >
            > The Post processor is a file that tells the software how to output the moves in Gcode format. Each machine has its own way it likes to see the gcode to run. There are sections of the post file that sets up the beginning of the gcode file and sections that setup the motion parts and sections that setup the ending of the gcode file. And there is the 'main' section that sets up the actual motion parts of the gcode file. The begging and ending parts can be the most important parts for they are the parts that set the machine tool into safe states for the start of motion.
            >
            > I would take a gcode file from your previous version and compare line by line with one from the new version and note the differences.
            >
            > inspect the post file to figure out, it can seem cryptic because of the C type of format, and see what is generating the line of gcode you want to change.
            >
            > Or better still, get a post from another user that has been altered for Mach, but you may want to learn how to edit a post yourself.
            >
            > As far as circle cutting, there are a few ways to tell a machine to cut an arc and Mach likes only one of those ways, I think. Look at the manual or on of the posted gcodes from when it worked.
            >
            > Hope this helps,
            >
            > Mark
            >
            > --- In mach1mach2cnc@yahoogroups.com, "steven_dantonio" <sdantonio93@> wrote:
            > >
            > > Hi,
            > >
            > > I'm making this inquiry on t unrelated forums at the same time. Also, I don't thing I can attach files to a post in a yahoo forum (at least I haven't figured out how to o it yet). I can send anyone the tow posts and the rhino file is anyone wants to look at them.
            > >
            > > I am a long time user of RhinoCAM 1.0 on Rhino (3 and 4) without any issues
            > >
            > > Recently I upgraded to Rhino 5 and finally installed RhinoCAM 2012 (lucky for me I kept the old Rhino 4 on the system).
            > >
            > > The steps I have taken and the issue is this:
            > >
            > > 1. I started Rhino5 (with RhinoCAM 2012) and made sure all the units were set to inches
            > > 2. I drew a test part (a circle and a square)
            > > 3. I set up 2 simple profiling operations and ran a simulation in RhinoCAM which worked fine (shown below as simulation)
            > > 4. I posted the results using Mach3-inch in RhinoCAM 2012 and got the file (g-code available if you want to see it)
            > > 5. I loaded it into Mach3, started up the system and tried a test cut, nothing moved.
            > > 6. I took the same part file and brought it up in Rhino4 (with RhinoCAM 1.0) and generated the following output (g-code available if you want to see it)
            > > 7 Set up the same test cut on the CNC and it worked perfectly as expected from looking at the g-code.
            > >
            > > In both cases I'm running RhinoCAM 4 and 5 on a Pentium 4, g GHz machine running WinXP SP3 (don't know if this is significant)
            > >
            > > The only response I got so far is (quoted below):
            > >
            > > "The only significant difference in the two G-code files is that the Rhino4 version is all done with G01 (directional commands at a feedrate) while the other uses G03 commands (move in an arc defined by I and J). This is a little trickier for Mach3 to interpret; make sure your postprocessor is in "absolute" mode for this sort of thing. You can also tell RhinoCAM to break down arcs into segments, as it was doing previously."
            > >
            > > When responding please consider me to be g-code illiterate, so, is this issue with the G03 commands something that can be solved at the mach 3 end or is it something that needs to be solved at the RhinoCAM end of things?
            > >
            > > Thank you,
            > > Steven
            > >
            >
          • Steve Blackmore
            ... Correct ... Mach3 handles IJ curves fine?? ... Steven- Mach3 handles curves fine, what you were told was bull. If Mach didn t move there is something wrong
            Message 5 of 9 , Mar 24, 2013
            • 0 Attachment
              On Sun, 24 Mar 2013 14:35:48 -0400 (EDT), you wrote:


              >I'm interested in this one too. I'm g-code illiterate as well, but I
              >understand that I and J commands make smooth curves making a machine faster and
              >smoother. That's worth upgrading RhinoCam.

              Correct

              >You seem to have found Mach 3 can't handle this... is this right guys?
              >I'm guessing Mach 4 will...?

              Mach3 handles IJ curves fine??

              >"The only significant difference in the two G-code files is that the
              >Rhino4 version is all done with G01 (directional commands at a feedrate) while
              >the other uses G03 commands (move in an arc defined by I and J). This is a
              >little trickier for Mach3 to interpret; make sure your postprocessor is in
              >"absolute" mode for this sort of thing. You can also tell RhinoCAM to break
              >down arcs into segments, as it was doing previously."

              Steven- Mach3 handles curves fine, what you were told was bull.

              If Mach didn't move there is something wrong with the Gcode. Post the
              Gcode up to and including the first G2 or G3 move.

              Fact - identical toolpath, one test using short line segments and one
              using arcs and arc approximation. Same feed rate.

              The segmented code took over twice as long to machine..

              Steve Blackmore
              --
            • Steve Blackmore
              ... If Mach gives this error Radius to end of arc differs from radius to start Line 22 on the line above. Go to general config, and alter IJ mode to inc - it
              Message 6 of 9 , Mar 24, 2013
              • 0 Attachment
                On Sun, 24 Mar 2013 22:07:01 -0000, you wrote:


                >G03X0.1250Y2.2663I-1.2308J0.9105

                If Mach gives this error

                Radius to end of arc differs from radius to start Line 22 on the line
                above.

                Go to general config, and alter IJ mode to inc - it should work then.
                (it does here)

                Steve Blackmore
                --
              • quadconversions
                Thanks Steve, Up till now I ve only ever machined huge organic shapes out of model board (car fenders, side skirts) and from a finish point of view it didn t
                Message 7 of 9 , Mar 24, 2013
                • 0 Attachment
                  Thanks Steve,

                  Up till now I've only ever machined huge organic shapes out of model board
                  (car fenders, side skirts) and from a finish point of view it didn't
                  matter. But, today I cut my first round pocket in aluminum to test my new bench
                  top router and you can clearly see the facets as the old RhinoCam g-code
                  tries to stitch together a radius. Smoother cuts and reduced cutting time
                  sounds like the way to go.

                  Regards Dave K


                  In a message dated 24/03/2013 11:20:29 P.M. GMT Standard Time,
                  steve@... writes:

                  On Sun, 24 Mar 2013 22:07:01 -0000, you wrote:


                  >G03X0.1250Y2.2663I-1.2308J0.9105

                  If Mach gives this error

                  Radius to end of arc differs from radius to start Line 22 on the line
                  above.

                  Go to general config, and alter IJ mode to inc - it should work then.
                  (it does here)

                  Steve Blackmore
                  --


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

                  www.machsupport.com - Web site AccessYahoo! Groups Links






                  [Non-text portions of this message have been removed]
                • Terry Wellman
                  Steven, What Steve is telling you should work. I ve got Rhino 5 64 bit running the latest version of RhinoCam 2012 4 axis. As I type, I m actually cutting my
                  Message 8 of 9 , Mar 24, 2013
                  • 0 Attachment
                    Steven,

                    What Steve is telling you should work.

                    I've got Rhino 5 64 bit running the latest version of RhinoCam 2012 4 axis.
                    As I type, I'm actually cutting my first parts with the latest download
                    from Mecsoft for 2012 4 axis. No problems so far (knock on wood).

                    The only other thing that I could think of would be if you had the wrong
                    post set up in RC2012 but the machine would still move, just not
                    necessarily the way you would want it to.

                    If you want, you can send your file to me at scmwcad1@... and I can
                    take a look at it. I'm working on a fun project for myself tonight so I
                    have some time to mess around.

                    Best,
                    Terry Wellman


                    On Sun, Mar 24, 2013 at 6:20 PM, Steve Blackmore <steve@...> wrote:

                    > **
                    >
                    >
                    > On Sun, 24 Mar 2013 22:07:01 -0000, you wrote:
                    >
                    > >G03X0.1250Y2.2663I-1.2308J0.9105
                    >
                    > If Mach gives this error
                    >
                    > Radius to end of arc differs from radius to start Line 22 on the line
                    > above.
                    >
                    > Go to general config, and alter IJ mode to inc - it should work then.
                    > (it does here)
                    >
                    > Steve Blackmore
                    > --
                    >
                    >


                    [Non-text portions of this message have been removed]
                  • steven_dantonio
                    Hi Steve, It worked perfectly, thank you. Steven
                    Message 9 of 9 , Mar 25, 2013
                    • 0 Attachment
                      Hi Steve,

                      It worked perfectly, thank you.

                      Steven

                      --- In mach1mach2cnc@yahoogroups.com, Steve Blackmore <steve@...> wrote:
                      >
                      > On Sun, 24 Mar 2013 22:07:01 -0000, you wrote:
                      >
                      >
                      > >G03X0.1250Y2.2663I-1.2308J0.9105
                      >
                      > If Mach gives this error
                      >
                      > Radius to end of arc differs from radius to start Line 22 on the line
                      > above.
                      >
                      > Go to general config, and alter IJ mode to inc - it should work then.
                      > (it does here)
                      >
                      > Steve Blackmore
                      > --
                      >
                    Your message has been successfully submitted and would be delivered to recipients shortly.