[jpbldr]

I've had my machine for a few months now, a Probotix Comet. I've cut a number of projects, many things just to learn the CAD/CAM process from design to finished part(using Fusion360). Made a few errors, but have managed not to crash/break anything. When I began I taped a piece of 1" insulation foam to the table as a spoil board to give me a buffer for mistakes, and cut mostly thin stock like balsa, thin ply, and foam board sheets. I've also done some 1/2" MDF for laminating forms and 1/4-1/2" ply for patterns and simple text signs. I removed the foam spoil board today and drilled a grid pattern in the supplied board to install some t-nuts so I can clamp some bigger material and be sure it doesn't move.


Next things I want to learn/do...

- I need to learn how to edit g-code directly or change how the postprocessor does so. Running LinuxCNC, on a Probotix machine and using Fusion360 for CAD/CAM. Before starting a cut, I zero the x-y-z axis on the part origin with the cutting tool in the machine, normally with the z being the top of the stock. Then when I start the cut the spindle moves up, and the machine prompts me to load the first tool. This is where I'm not sure what I'm doing wrong, I already loaded the tool, and I just click through that prompt. It never engages the surface, stopping short in the z axis but continues to follow the cutting path otherwise. I then stop the cut, click the return to x-y zero, re-zero the z axis again, and restart, at which point it moves to the correct z position during the cut. Any pointers to g-code/postprocessor knowledge would be very welcome.


- Build some fixturing blocks, and clamps to use with the hole grid I have now. Plan is to use simple blocks to capture corners of rectangular stock and some cam clamps to grip the sides of the stock. These I will draw up and use the machine to cut them out. Probably will be some revisions involved. Also some hold down clamps of some sort.

- Build a vacuum table for cutting thin sheet stock. It isn't apparent in the builds or videos I've seen. Do people use a spoil board "insert" of some sort on the vacuum tables?

Very happy with the machine so far and looking forward to more projects.



Brian

 

[difalkner]

Which Post Processor are you using, Brian? I don't have a CNC Router Parts machine but that's the one I'm using and it works just fine with no wasted motion.

On the vacuum for thin parts I've seen many folks make a manifold with a grid pattern. Plenty of YouTube videos on that. I see a lot in the Luthier arena where folks are holding bridges, fingerboards, etc.

Larger operations just pull a vacuum through the MDF spoilboard but that takes some serious vacuum pumps, likely costing more than your CNC. But you could scale it down for small 'pads' of vacuum equipped MDF pieces, say 15"x15" or so, and maybe a smaller pump will pull through that but I haven't tried it so test first.

David

 

[MT Stringer]

Welcome aboard.

The last time I was at the local lumber yard in Houston, the guy gave me some scrap pieces of 1/8th inch baltic birch. These are the pieces that cover the top of the pallet when it comes to their yard. They just throw it away. So...I am using it as a spoil board to protect my bed. Being thin, it clamps easily and provides just enough extra protection so the spoil board doesn't get cut up.

Good luck and happy cutting.

 

[MoHawk]

Here is a link to G & M Codes. https://www.cnccookbook.com/g-code-m-code-reference-list-cnc-mills/
Evidently the PP your using is a ATC PP, auto tool change which stops the gcode so you can change the cutter. I would guess that your software will allow gcode editing. M06 is the code for tool change. Gcode is just a text file than can be opened in Windows Notepad to edit.

 

[MoHawk]

Here is a link to G & M Codes. https://www.cnccookbook.com/g-code-m-code-reference-list-cnc-mills/
Evidently the PP your using is a ATC PP, auto tool change which stops the gcode so you can change the cutter. I would guess that your software will allow gcode editing. M06 is the code for tool change. Gcode is just a text file than can be opened in Windows Notepad to edit.

 

[jpbldr]

Difalkner,
Im using the linuxCNC post, as that is what the machine is running. Are you saying you're using the CNCRP post with a machine running linux?


Mohawk,
CNCCookbook is where I've been learning so far.


I'll get it figured out slowly.


Brian

 

[honesttjohn]

For Post Processor try -- EMC2-G64Arcs (inch or metric)

 

[BalloonEngineer]

The g-code used by CNC routers is generally very simple, and many of the post processors will produce satisfactory code. The metal machine world has machines with many special functions that normally aren’t used on routers (coolant, rigid tapping, etc.) so the many machine specific post processors are to setup those kinds of features. Basically, only the first few lines, and last few are the differences, the others are the line numbering format, how many decimal places, capitalization, spaces between commands, etc. Some older machines required very specific formatting, modern control programs can parse almost any variations.

The CNC Router Parts machines generally run Mach, so their posts are very similar to the Mach ones, which are purposely very generic, since there are so many machines (and many kinds of machines) that run Mach. The “EMC” one that @honesttjohn suggested should work well, “EMC” was the original name for the software that eventually became LinuxCNC. He also runs a Probotix machine, so his advice is well-founded.

 

[jpbldr]

To clarify my previous answer, the post I'm using in Fusion is named LinuxCNC(EMC2). I left (EMC2) part off before. I believe this is the correct post processor.

I just looked and there is no option called EMC2 alone.

Here is a screen shot of where the machine stops (the line highlighted is where it always stops). I've read through the lists of codes before but this is my first real attempt to break it down line by line.



N10 - abs. zero XYZ, feed rate, select XY, incremental IJK - The first 3 are pretty simple, and I think I understand the IJK command as just an additional coordinate definition for how to handle arcs.
N15 - inches
N20 - machine coord sys. - this cancels work offsets?? but does that revert on the line 40 command?
N25 coolant off
N30 tool 1, tool change
N35 RPM, spindle on
N40 work coord sys
N45 coolant on - I normally disable that in my setup, maybe I forgot on this one
N50 rapid to XY

 

[jpbldr]

I added a few more lines from the file than what are shown in the screenshot. N20 is where it stops, even thought the tool change isn't called until N30.

Am I correct that the g53 command in this case is just to rapid to high Z position for the tool change and that is why it stops there? waiting for the tool change... But g53 also indicates that it cancels work offsets. Is this what is causing my Z error until I rezero Z?


Brian

 

[4DThinker]

The prompt to load a tool is normal. When linuxCNC is first started up it has no tool info. So when you load/run your first file it finds the first tool number reference in that file and issues the prompt. If you already have a tool in place then just hitting Continue is OK. It is in there to help remind you to have the needed bit in place.

Your bit starting out too high may be from where you set the origin point in Fusion 360 before saving the toolpaths. If you built your project/sketch above (up) from where Z=0 then you likely need to set Z Zero in linuxCNC on the spoilboard rather than on the top of the material. There may be an option in Fusion 360 to change that Z origin reference while creating your toolpaths.

I have a copy of but don't use fusion 360 to make my toolpaths. I use Aspire from Vectric. To me their CAD/CAM products more logically proceed from setting up your material through saving the toolpaths. IMO Fusion 360 is trying to be everyman's CAD/CAM, including for 3D Printing. As such it does far more than you actually need for most CNCing. That confuses me, and I'm very experienced making things on my Probotix Meteor.

You can download free trial versions of Aspire or VCarve Pro or Cut2D from vectric.com. They won't let you actually save/cut any but the included demo files, but should give you an idea how they work. Many tutorial videos also on their site.

4D

 

[difalkner]

Difalkner,
Im using the linuxCNC post, as that is what the machine is running. Are you saying you're using the CNCRP post with a machine running linux?

Brian

No sir, I'm running Mach4. Sorry for the confusion.

David

 

[jpbldr]

The prompt to load a tool is normal. When linuxCNC is first started up it has no tool info. So when you load/run your first file it finds the first tool number reference in that file and issues the prompt. If you already have a tool in place then just hitting Continue is OK. It is in there to help remind you to have the needed bit in place.

Your bit starting out too high may be from where you set the origin point in Fusion 360 before saving the toolpaths. If you built your project/sketch above (up) from where Z=0 then you likely need to set Z Zero in linuxCNC on the spoilboard rather than on the top of the material. There may be an option in Fusion 360 to change that Z origin reference while creating your toolpaths. 4D

4D,

The initial prompt makes sense, I agree. Fusion, in CAM workspace, does allow you to set the origin point and axes of the toolpath, separate from the model origin and axes. With few exceptions, I have always set that (CAM origin) at the front left corner of the work piece for XY. The Z I have tried both ways, top of work or top of spoilboard. The result is always that the first try either doesn't even touch the material (say, 1/16" stock where I'm only doing a single pass), or, on thicker stock where I'm making multiple passes, the first pass(+) don't make contact and the final pass while it may have been cutting is not at the correct depth(too shallow). Then, if I simply reset the Z zero, to the same exact point I did originally, and restart from the beginning, the cut will be correct. I am not changing the toolpath via Fusion, and reposting. Only rezero the Z , and press the start button again. Same exact .ngc file that came out of the postprocessor to begin with, different result after resetting Z.



Brian

 

[Jeff Speedster929]

You can take the G53 line out. Also the M9 and T1M6. M9 is coolant code and M6 is tool change. You only have one tool so no need for the extra commands.

 

[4DThinker]

If it takes a new resetting of the Z origin, then I suspect you haven't actually set it the first time you thought you did. This happens to me occasionally when someone distracts me while I'm setting up a cut. I've move the bit to my material top, but forget to actually tell linuxCNC (click on Set Axis Origin). You need to be sure that Z is the axis selected when you do this.

I've also gotten into the practice of issuing (in the MDI tab) a G0X0Y0 command, followed by a G0Z0 command after I've set all my origins. This should move the bit over to and down to where all your origins are set. When the bit doesn't end up where I think it should go, it is always because I forgot to actually click on Set Axis Origin.

Your machine is newer than mine though. Your linuxCNC install is newer than mine. Probotix may have introduced a bug in their configurator. They've been updating it quite a bit lately. Maybe it's a feature we just don't understand. My only frame of reference are the three Probotix CNCs I oversee, and I've never seen them do what you describe. When Z isn't where I thought it should be, it has always been my fault in forgetting to set it.

4D

 

[jpbldr]

I may have found the issue. And I should have called Probotix in the first place.

Edited the tool.tbl file in Probotix application to make all tool lengths 0. The tool 1 length was set to .5, which corresponds to the error I was seeing.

I will have a chance to run the machine tonight and will report if this is the fix.


Brian

 

[jpbldr]

So, I ran several different cuts tonight. Some from existing files I've run before, some from new files.

Since the problem I was having was only an issue on the first cut after machine bootup, before the (tool 1) command, I completely shut down the machine and restarted each time to confirm the fix. The tool.tbl file is what was causing the Z offset. I do not have the Atlas tool sensor that Probotix offers, and this may be a file specific to that. I edited that file so that all tools have a "0" length.

Happy! that Probotix tech support answered phone on the second ring, and Caden (sp??) quickly pointed me to what was causing the issue and how to resolve it.


Brian

 

[honesttjohn]

Caden is good. We've become best friends this week after all the time on the phone. Nice to be able to talk to a live person and not be rushed.