Official Luthiers Forum!

I finally got my Laguna IQ Pro installed and running. I'm using Rhino3d with MecSoft's RhinoCAM. Things are going OK, but I'm running into a problem every time I try to do lettering with a vee bit. Here's what I'm doing and the problem:

1) I create the part in Rhino3d, including some lettering. To create the lettering, I use the TextObject command, and I place the lettering at the top surface of my part. It all looks good in Rhino3D.

2) I then generate the toolpaths using RhinoCAM 2014 in the Machining Browser. For the lettering, go to the Program menu, select 2 Axis, and V-Carving. I select the text objects as my drive regions. I edit the tool to be the same as my v-bit. Under Cut parameters, I have selected the cut side as "inside", location of cut geometry as "At top," and the total cut depth is 0 by default. (I've experimented with other values for cut depth and have the same problems.)

3) I generate the toolpath and simulate it. It looks fine.

4) I post the lettering operation to a USB stick and take it to my IQ Pro. I touch off the tool, load the lettering program, and tell it to run. The Spindle goes to the home location and stops. I get an error called "axis error." It won't cut the letters.

I have no idea what I'm doing wrong, but I've tried it with multiple parts and always have the same problem.

Any suggestions?

The simulation usually matches quite well to real life. I'm guessing there's either something wrong with your post processor or maybe your clearance plane is out of axis range or something like that. MecSoft can help you with the post processor.

If you post the first 50 to 100 lines of G-code it might be easier to give some feedback.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Thanks, Andy! I'll post some GCode tonight when I get home.

Here's the first 100 lines of GCode. It's completely Greek to me.

N1 G00 G17 G40 G90
N2 G70
N3 G54
N4 (Lettering)
N5 T2 M06
N6 D2
N7 M03 S18000
N8 G00 X-3.0004 Y6.5000
N9 G00 Z0.4600
N10 G01 Z0.2120 F29.3
N11 G01 X-2.9722 Y6.5194 Z0.1926 F40.0
N12 G01 X-2.9447 Y6.5945 Z0.1939
N13 G01 X-2.9426 Y6.6002 Z0.1936
N14 G01 X-2.9386 Y6.6065 Z0.1921
N15 G01 X-2.9345 Y6.6112 Z0.1899
N16 G01 X-2.9249 Y6.6081 Z0.1946
N17 G01 X-2.9227 Y6.6074 Z0.1950
N18 G01 X-2.9157 Y6.6066 Z0.1957
N19 G01 X-2.8157 Y6.6068 Z0.1959
N20 G01 X-2.8086 Z0.1955
N21 G01 X-2.8019 Y6.6082 Z0.1941
N22 G01 X-2.7931 Y6.6114 Z0.1898
N23 G01 Z0.4600 F11.0
N24 G00 X-2.7533 Y6.5194
N25 G00 Z0.4600
N26 G01 Z0.1926 F29.3
N27 G01 X-2.7822 Y6.5940 Z0.1939 F40.0
N28 G01 X-2.7847 Y6.6005 Z0.1936
N29 G01 X-2.7888 Y6.6067 Z0.1921
N30 G01 X-2.7931 Y6.6114 Z0.1898
N31 G01 Y6.6184 Z0.1924
N32 G01 X-2.7944 Y6.6259 Z0.1940
N33 G01 X-2.7981 Y6.6352 Z0.1944
N34 G01 X-2.8279 Y6.7109 Z0.1945
N35 G01 X-2.8406 Y6.7447 Z0.1953
N36 G01 X-2.8509 Y6.7733 Z0.1964
N37 G01 X-2.8542 Y6.7795 Z0.1956
N38 G01 X-2.8555 Y6.7813 Z0.1951
N39 G01 Z0.4600 F11.0
N40 G00 X-2.8440 Y6.7982
N41 G00 Z0.4600
N42 G01 Z0.2120 F29.3
N43 G01 X-2.8555 Y6.7813 Z0.1951 F40.0
N44 G01 Z0.4600 F11.0
N45 G00 X-2.8870 Y6.7982
N46 G00 Z0.4600
N47 G01 Z0.2120 F29.3
N48 G01 X-2.8753 Y6.7812 Z0.1950 F40.0
N49 G01 Z0.4600 F11.0
N50 G00 X-2.9345 Y6.6112
N51 G00 Z0.4600
N52 G01 Z0.1899 F29.3
N53 G01 X-2.9346 Y6.6181 Z0.1925 F40.0
N54 G01 X-2.9334 Y6.6256 Z0.1940
N55 G01 X-2.9299 Y6.6350 Z0.1944
N56 G01 X-2.8895 Y6.7434 Z0.1948
N57 G01 X-2.8799 Y6.7730 Z0.1964
N58 G01 X-2.8769 Y6.7790 Z0.1957
N59 G01 X-2.8753 Y6.7812 Z0.1950
N60 G01 X-2.8688 Y6.7826 Z0.1964
N61 G01 X-2.8619
N62 G01 X-2.8555 Y6.7813 Z0.1951
N63 G01 Z0.4600 F11.0
N64 G00 X-2.7669 Y6.5000
N65 G00 Z0.4600
N66 G01 Z0.2120 F29.3
N67 G01 X-2.7533 Y6.5194 Z0.1926 F40.0
N68 G01 X-2.7246 Y6.5000 Z0.2120
N69 G01 Z0.4600 F11.0
N70 G00 X-2.9584 Y6.5000
N71 G00 Z0.4600
N72 G01 Z0.2120 F29.3
N73 G01 X-2.9722 Y6.5194 Z0.1926 F40.0
N74 G01 Z0.4600 F11.0
N75 G00 X-2.6584 Y6.5000
N76 G00 Z0.4600
N77 G01 Z0.2120 F29.3
N78 G01 X-2.6765 Y6.5181 Z0.1939 F40.0
N79 G01 X-2.6946 Y6.5000 Z0.2120
N80 G01 Z0.4600 F11.0
N81 G00 X-2.5917 Y6.6760
N82 G00 Z0.4600
N83 G01 Z0.2120 F29.3
N84 G01 X-2.6027 Y6.6994 Z0.1934 F40.0
N85 G01 Z0.4600 F11.0
N86 G00 X-2.5789 Y6.7097
N87 G00 Z0.4600
N88 G01 Z0.2120 F29.3
N89 G01 X-2.5984 Y6.7017 Z0.1966 F40.0
N90 G01 X-2.6027 Y6.6994 Z0.1934
N91 G01 X-2.6102 Y6.7008 Z0.1929
N92 G01 X-2.6186 Y6.7011 Z0.1928
N93 G01 X-2.6249 Y6.7004 Z0.1936
N94 G01 X-2.6301 Y6.6985 Z0.1944
N95 G01 X-2.6340 Y6.6963 Z0.1950
N96 G01 X-2.6420 Y6.6903 Z0.1977
N97 G01 X-2.6438 Y6.6889 Z0.1981
N98 G01 X-2.6502 Y6.6812 Z0.1995
N99 G01 X-2.6555 Y6.6747 Z0.2004
N100 G01 X-2.6610 Y6.6692 Z0.1982

Some additional info:

After I try to run the program and the machine goes to the home position, I can go under the "Alarms" screen on my controller, and it shows the following errors:

Under "CNC Alarms," it shows:
Target Position > Positive SW End (G00, G01)
Axis Index 2
Program Number -1
Blocknumber N9

Then also under "CNC Alarms:"
No text found for error number 7746

Then also under "CNC Alarms:"
NC Program aborted by axis error
Axis Index 0

I don't know what any of this means.

The G-code looks all normal and fine to me. I'd call up laguna on this one - it would be fastest.

The alarm info is most helpful. N9 is the line number. If we look at N9:

N9 G00 Z0.4600

G00 is a rapid move, Z axis to ).4600. The alarm is saying that where you're commanding the machine to go is greater than where it can go or something like that.

Best guess is that you're doing something incorrectly when setting Z-zero of your work piece on the machine or possibly there's something wrong with where you set your work zero in RhinoCAM. i.e. something is different between where RhinoCAM is thinking Zzero is and where you're actually setting Zzero.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

Andy, thanks for the great response.

I sent an e-mail to Laguna this morning, and they got back to me right away. I'll try their suggestions when I get home tonight. I'm going to write all of this up here in this thread, in the off chance that someone ever has this problem and finds it helpful. (Or, more likely, that I have the problem again in a couple years and can't remember what the solution was.)

Laguna's customer service guy points out that N5 calls for T2, which is expecting my machine to have an auto tool changer so that it can change to tool 2 automatically. But my machine doesn't have an auto tool changer, so that doesn't work. So I need to go into RhinoCAM and edit the vcarve bit to be tool 1 instead of tool 2, which will take the tool change operation out of the gCode. (Alternatively, I could buy an auto-tool-changer. But the software approach is a bit cheaper.)

I never would have figured that out on my own!

With that said, he also agreed that the N9 error indicates that z0.46 in line N9 is out of range. My hunch is that this issue is an artifact of the tool changer issue. Specifically, I suspect the controller believes I have a tool changer, and believes that once the tool changer switches to the v-bit, I'm going to have some big long bit that won't be able to go to z0.46. I'm hopeful that, once I correct the tool changer issue and touch off the v-bit, the controller will no longer think z.046 is out of range. We'll see. I'll post my results after I get a chance to try it out tonight.

That's true...kind of. You should ask Laguna or check in the manual about how exactly they recommend dealing with tool changes without a tool changer. With my setup, I can either set the machine to ignore M6's in the code (it stops until you hit cycle start again) or, when it comes across an M6, it moves to a tool change position, I change the tool, and then it goes to a fixed touch off plate to measure the tool length.

Ask them what line N6 D2 is while you're at it....never heard of that.

If an ATC is available for your machine, it is possible that is has built in offsets of some sort already in the tool table by default.

_________________
http://www.birkonium.com CNC Products for Luthiers
http://banduramaker.blogspot.com

I will find out about ignoring the tool change codes.

In the meanwhile, editing the tool to be tool 1 instead of tool 2 fixed the problem. I was able to vcarve letters no problem.

My first project has been a template for my Robbie O'Brien Neck Angle Jig. The template is for a dovetail on a neck for a Benedetto style archtop. (He uses a weird dovetail style.) Here are some photos. I'm super happy with how it came out. Apart from the template being extremely precise, I was able to vcarve the label and the instructions to tell me what bit and router guide bushing to use. You can see that the template is much finer workmanship than the rest of my work on the jig (done without the benefit of CNC)! This tool is going to be a great benefit and improvement to my work. Thanks for all of your help!

I was going to say to try changing the T2 to T1...or deleting it from the line entirely....but it looks like you got it.

Also go into the Rhino software and take a look at your tool selection process. The T2 command could not have been generated by the post processor unless you had inadvertently changed it from the default in the software when you were making your tool paths and selecting tools. It might have happened, for instance, if you have selected a tool and then changed your mind and selected another one instead. It might have automatically assigned the follow up choice as tool #2 and maybe you forgot to change it back. something like that.

_________________
I read Emerson on the can. A foolish consistency is the hobgoblin of little minds...true...but a consistent reading of Emerson has its uses nevertheless.

StuMusic