[sdantonio]

Hi,

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 (shown below as part)
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 (shown below as Part (RhinoCAM 2012_Rhino 5).txt)
5. looking at this file it is not going to run much of anything, to make sure I loaded it into Mach3, started up the system and tried a test cut. As expected nothing moved.
6. I took the same part file and brought it up in Rhino4 (with RhinoCAM 1.0) and generated the following output (shown below as Part (RhinoCAM 1.0_Rhino 4).txt)
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

Anyone seen any issues that are remotely like this or have any suggestions as to what may be happening?

Thank you,
Steven

[awerby]

It's difficult to understand what your problem is from what you're sharing here. The only difference I can see in your screenshots is that one has the regions highlighted but the other one doesn't, but I'm not sure if that's significant or not. Did it start but stop with an error message? 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.

If none of this helps (and nobody else is able to explain it better before Monday) you're fortunate to be using such a well-supported program as RhinoCAM. Just call Mecsoft and the tech support guy will be able to use GotoMeeting to get inside your computer and show you exactly how to fix your problem.

Andrew Werby
www.computersculpture.com

[sdantonio]

Hi Andrew,

Thank you, Ill have to look into your suggestions. One thing I noticed, and I don't know if it is of any significance, then I deign a simple part from scratch in rhino5 and generate a post from this it generates using G01. if I load or import a rhino4 file and then generate a post from it I get the post generated using G03 commands. I'll have to try forcing the system to generate using G01 as you suggested and see what happens.

Thank you for your input. I'll keep you posted as to what I get for files.

Steven

[sdantonio]

Hi Andrew,

Now that I'm digging into the post I'm wondering if I am implementing your suggestions correctly. The post seems to be set to absolute already and I set the circles tab to absolute instead of predefined "vector from start to center". I don't see any difference on the post output (or am I digging around in the wrong section of the software?)

I've attached two more jpegs to show where I am in the post editor (of course when I saved the edited post I saved it with a unique name rather than overwriting the original file in the event that I an in the wrong area to implement your suggestions).

Steven

[awerby]

Hmm, that seems like it should have worked. (I was talking about the absolute settings in the Circles tab). Since apparently it didn't, could you call up Mecsoft tech support tomorrow and ask them what you did wrong? Then post back to this thread and tell us what you had to change to get the G02 and G03 commands working correctly in Mach3.

In the meantime, to set it back to the way it was in Rhino4, go to the toolbar on top of the RhinoCAM browser window. In Machining Operations/ CAM system Preferences/Machining Preferences, click the box that says "Output arcs as linear segments." This should change all the outputs to G01, the fineness of the segments determined by the tolerance settings in Rhino.

Andrew Werby
www.computersculpture.com
.

[sdantonio]

All Andrew,

Apparently Mach3 does support G03 commands (I also spoke to some of the MAch3 developers over the weekend).

I implemented the following instructions and it worked fine:

in mach 3 general config setup modals have a play with distance mode and IJ mode Absolute or inc (pic attached)

one will give a stop and go at the end of each line or spline and the other will run straight through


This may have been the same thing you said, but in this case the pic helped immensely. No changes needed to be made to either Rhino3d or RhinoCAM 2012

Thank you for your help,
Steven

[sdantonio]

It occurred to me after posting this that I should have also included Steven Blackmores instruction set

> >G03X0.1250Y2.2663I-1.2308J0.9105 <-- this is where Mach3 would just to and then stop dead
>
> 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

Steven