Pocket NC 5-Axis Coordinates

[Anonymous]

My company was one of the lucky first recipients of the new Pocket NC desktop 5-axis mill. I'm having trouble setting up parts so that the gcode makes sense to the machine. I talked to Matt, of Pocket NC, and he cleared up some things, but every program I post to the machine throws up errors about exceeding the machine's travel. I know the toolpaths are safely within the envelope of travel, but I think there's an issue with the orientation of the origin in the CAM setup in Fusion. I'm using the bed/vise model that Pocket NC released, which includes the point of rotation for the A and B axes. Autodesk's Ehren Lundgren suggested that, since Autodesk and Pocket NC have partnered, I might be able to find some guidance here. Any help or direction would be hugely appreciated.

[Steinwerks]

What's your clearance plane? Does the machine use tool length offsets (I assume it does)? You might want to share some snippets of code too.

[AchimN]

Can you please share your nc-program also?

[Laurens-3DTechDraw]

---

@AchimN wrote:

Can you please share your nc-program also?

---

That would also answer my question, is the coordinate system at the top in the middle?

But another one would be; And how is this point set in the workoffset on the machine?

[Anonymous]

The machine does use tool-length offsets, though at the moment, I only have one tool entered in the table. The origin is set in Fusion at the point of rotation of the A and B axes, based on a model provided by Pocket NC. This point corresponds to the home position of the machine so that, in theory, one shouldn't need to set work offsets before running a part. This point is .885" above the machine bed, in the middle of the B axis. Here is their page detailing travel and home positions: http://www.pocketnc.com/home-position

[Anonymous]

Here is a more complete package to diagnose. The zip file has the F3D file, gcode, and a screenshot from the controller showing the error in the lower right corner.

[Steinwerks]

I think there are a few issues with your setup with regards to how the machine is expected to move, so I am altering some things and will share it here when done. Also I'd be using a 3D Adaptive toolpath for your roughing strategy, much more efficient, especially with the machine being so small (lack of rigidity).

[Steinwerks]

I've made a few changes with regards to tool orientation and some Setup changes based on the Pocket NC description of the machine, which is lacking a bit in terms of what the table looks like at home position. Most 5-axis machines of this sort of construction have the spindle orientated vertically to the table whereas the photos in your link have it oriented more as a HMC would be, so I find this a little confusing. This initial setup is critical, of course, so you don't just start cutting your table apart or crash the head into your workholding (not that it moves real fast, but you get the idea).

After that it can all be aligned with Tool Orientation. Take a look at the attachd file and let me know if it's helped at all. I don't see anything in the NC file that pops out, but your error suggests it's not even in a Z move (line 686 is this one if the shot is to be believed and line 1 is the % sign: N3425 X0.3864 Y-1.5374 ).

[Anonymous]

I see what you mean about the adaptive clearing. Unfortunately, the toolpaths from your modified file are creating the same LinuxCNC error. I had heard that Autodesk has a Pocket NC at Pier 9 which, if true, might mean that somebody on the Autodesk staff has successfully programmed parts on it and might be able to troubleshoot my problem.

[Anonymous]

It looks like part of the problem is that the LinuxCNC control software is skipping to the middle of the program (and risking a crash) when told to "go". I had a similar problem running a Tormach 770 mill a couple of years ago, but that used Mach3 and was the result of tool names and operation names that registered as comments. As a result, it would skip to the end of the NC file, looking for vaild code. I can't figure out what might be happening in this case, though.

[AchimN]

So by looking into the picture attached your machine looks like a horizontal machine.

If this is true, the initial Z-direction of your initial WCS in Fusion is wrong.

You would need A+/- 90 deg to machine the part is that right?

[Anonymous]

That's correct. I fixed the initial origin orientation so that the gcode instructs the machine to rotate A 90 degrees. The controller software now jumps arbitrarily to line 1019 of the program, skipping the A axis command and risking a crash.

[RandyKopf]

Does your setup WCS Coordinate system match Pocket NC's default homing origin? 

The coordinate system you show is fine for the tool path itself but I don't see the SETUP WCS origin.

When Pocket NC Homes it is at X+2.500 and Y +2.500. So if the But the Rotary Centerlines are .885 up in Y

So take Y+2.500 and subtact the .885 Value and the max clearance you can have is Y+1.615 above the WCS. 

I may be off on a tangent... Since Pocket NC is shipped out of the box with no current Fixture offset support in 5 Axis mode you must use the origin of the machine when it is homed. Next you must set your part up with literal values. This is a bit backwards compared to modern 5 Axis CNC's using TCP or Fixture Compensation but it does works. 

The three images below explain the SETUP WCS to Tool Path CYS correlation on Pocket NC.

1) In the first photo you see the Pocket NC at it's home postion. In the example the PNC vise is oriented from Center to the Right. That is along the X Axis on the right side of the rotarty centerline. (Notice the Z Axis Blue Arrow shows the positive direction that the Z Axis moves in when the machine is homed.)

2) The second photo shows the Fusion 360 CAM SETUP Screen. Notice the Z Axis matches the actual Pocket NC's Z Axis when it is homed.

3) The Third photo shows an engraving tool path. But notice it's Z Axis is now pointing upward. (See the Blue Z Axis Arrow.)  It is the direction the tool needs to approach the part and cut it. 

But also notice that within the dialog box for the Engraving tool path the origin is specified as WCS. That is making a hard reference to the Z Axis that is used in the SETUP. Now the post can tell that starting out Z needs to be output with respect to the WCS and the Pocket NC Post is setup so that is A0 B0. Next when the tool path is processed the post sees that the engraving Tool Z Axis orieintation is now in a different direction. And it outputs A90 B0 so the tool path will move the PNC Rotary Tables correctly. All the clearance planes etc need to be hard set with respect to the math of the PNC. 

Message me if you need futher explanation.

Randy Kopf

[Anonymous]

Hi, I'm interested in purchasing a pocket nc for my employer and I'm trying to find out as much about it as I can.  I saw in your post a jpeg image of the A or B axis with the gear teeth.  Do you have a 3D CAD model of that that you could share?  

Christine