RhinoCAM / Fusion 360 post processors

1

Hi all, and thanks in advance for any answers…
I’ve found a similar forum topic, but not exactly the same problem, so here goes:

I’m brand new to this, and in the first stages of trying to learn my new machine (5x5, EX controller, cnc12, nema 34’s, 4hp spindle, no 4th axis).

I’ve been trying to find any simple, pre-made files to run as tests, while I figure out the machine operation and try to find my way through the design process in the free trials of Vcarve, Rhino/RhinoCam and Cut3D. While Vcarve is supposed to be simple, but I’m not getting anywhere with it, it doesn’t give a compatible post processor option. Cut 3D seems to offer the most reasonable free test files, and I’ve had some success, but keep running into the same stubborn error over and over:

I think my initial setup went well: homed, squared, Tool height setter calibrated and top of spoilboard calibrated. Tool measured by MTC, part zeroed using the
touch plate utility. That sets up WCS #1 as X=0, Y=O and Z=2 (when the bit is indeed 2" above the stock surface) and all seems well.

Then I’ll load the job and run the rough pass successfully with a 1/4" end mill. Get prompted for the tool change, change to 1/4" ball nose bit for the finishing pass, continue through spindle start and the fun begins - the machine comes straight down in the home position with the spindle running, touches the tool setter plate (which I’m pretty sure it’s not supposed to), and rapids off to the workpiece at 5mm above the spoilboard surface and burrows into the side of the stock. I’m getting familiar with the Estop.

I’ve run this several times in a few different ways with 2 different projects, same result. I’ve tried separating the rough pass and finish pass files, same result. I’ve cleared worholding out of the way (because I’m getting familiar with where and when it’s going to go) and let it keep running a bit, and it seems like it will continue cutting lower and into the spoilboard as it begins running the finishing operation.

When I start the run cycle, I get a “Z axis limit exceeded error” message flash, then it starts. The Gcode line error checks out to be the line right after the tool change, but the Z value looks to be correct (5mm, which is the clearance value I entered in the Cut 3D setup).

Any ideas? How come the rough pass works fine, but the finish pass thinks the top of the stock is at the spoilboard height?

I’m sure this is my error, but I can’t seem to solve it.

Again, thanks for anyone’s advice!

Grant

2

Avid’s Vectric Posts: Vectric - CNC Software

Sounds to me like a post issue. EX controllers have to be used with the correct post processor.

3

EX posts are built into VCarve, if they aren’t they can be downloaded here:

https://www.avidcnc.com/support/instructions/software/downloads/vectric/

Only download these if you cannot find them in Vcarve

Sounds like you got that all right, nice!

I think all of your trouble here is not using the right post processor. What it IS supposed to do is this:

Run the job with the first tool, when it gets to the second tool it’s supposed to prompt you and then head over to the tool height setter. You then swap the tool and press cycle start. The tool will get measured. The machine will then move ALL THE WAY up in Z and rapid back to where it’s supposed to cut, drop down into the cut and keep cutting.

If you’re not seeing this behavior I’m certain it’s because you’re not using the right post.

Also EVEN if you’re using the right post you need to make sure that in your material setup in VCarve you have your heights for rapids and plunges set properly. That could cause you cut into your material when moving around the table too.

This is likely back to the improper post you are likely using. In posts that are not ours tool “tool length comp” gets cancelled (and it shouldn’t) this means that the controller doesn’t know the height of the tool, and when you go to run a job you get those errors.

Moral of the story here is use the right post and your problems will be gone :slight_smile:

4

Hi Eric,

Thanks for the quick response.

I’d like to say I’ve got it solved, but it’s just the opposite. Problems on top of problems.

You’re absolutely right, the Gcode generated in the Cut3d free trial test files contains lines that say " tool height compensation cancelled", so I guess that means that it can’t output information that the EX controller/Centroid likes… even though their site says my machine is supported, and it seems to be a Vectric product. I’ve reached out to them but haven’t heard back yet.

So, I’ve spent the day working with the Vcarve pro free trial, and again, no luck. The only test file they have is the “welcome sign”, and when I work through it and output a toolpath, I get the same error message before cycle start, “Z axis travel exceeded, line xx”.

I’m also getting erratic behavior from the machine: while jogging I accidentally hit up instead of down, and it thumped into the Z axis top stop/sensor (didn’t think it should be able to do that) and got frozen because the sensor light couldn’t disengage. I thought it was something wrong with my assembly: removed the sensor, manually jogged away from the sensor location, and reset the sensor height. Proceeded to home, and it thumped into the Y axis bumpers/sensors and got similarly stuck. Power cycled it all, carefully reset all sensor locations and it seems to be able to home now, but what happened? I’m reluctant to try to jog to the end of the soft limits again because the crash is pretty forceful. It seems to be able to home itself again now.

And on a recent attempt to run the Vcarve test project, I set the material XYZ zero with the touch plate, glanced back a minute later and the WCS Z location was reading 0 at the top of the Z axis, not the usual 12" or so. Like it was confusing WCS locations with the MCS. Am I correct that home MCS is 0,0,0, and that is front left, top of the Z axis. A WCS gets a 0,0,0 at the chosen top corner of the stock (this’ll be front left top of stock for me, so far.)

Trying to make sense of it, I may not be explaining it well enough, but the machine seems buggy on the Z axis, both mechanically and programming wise.

I have to commit to buying one or other software system, it would sure be nice to know if the Z axis problem is coming out of the CAM, post processor or the cnc12 itself.

Thanks again for any input!

Cheers,

5

You are using the wrong post processor. You need to use the Avid EX post. As I said earlier this is the root of your problems

The posts are available right in Vectric. You just select them from the list of posts in your machine setup

You can find instructions on how to setup a machine, and associate post processors here:

https://docs.vectric.com/docs/V11.5/VCarvePro/ENU/Help/form/tool-database-machine-management/index.html

You need to pick the “Avid EX” post from the list. If you do not do this you will get G code that is compatible and will cause issues.

You should not be able to do this. Are you using CNC12 software downloaded from our site? Or are you using another version of CNC12?

Are you running the “Avid profile manager” to launch your CNC12 profile?

Jogging up past the Z limit shouldn’t be possible unless you are not running our software or have one into the motor settings and tried disabling limits…

12" is not usual. If the tip of your bit is on top of the material that you’ve used the touch plate on it should say 0 for Z.

Please start with the correct post and work from there. This is the source of your issues.

6

Hi Eric,

Thanks.

As far as I know, I’m following the assembly and setup instructions. CNC12 downloaded from your site, and Avid profile manager.
I haven’t gone into any advanced settings and disabled or changed anything…

I heard back from cut3d re the post processor. Being new to this I didn’t realize cut3d was a “legacy” product and effectively out of date. Although their info lists the Avid 5x5 pro with EX and Centroid as supported, that is not currently true. I already own Rhino and was hoping to design in Rhino, Cam in Cut3d and be done, but it looks like that’s not possible.

Let’s look at this differently: CAM choices are limited to Vcarve, Aspire or Fusion360?

I can get the Vcarve test “welcome sign” to run, but I’m reluctant to purchase the software. It’s clearly not aimed at 3d work. Aspire is a big step up in cost yet still seems limited in its 3d ability.

Do you know if RhinoCam has a working post processor for the current EX/Centroid/CNC12 configuration?

Cheers,

7

We have posts for “legacy” Vectric products if you want to use them

Someone has a Centroid post out there: https://www.cnczone.com/forums/rhinocam/353514-cnc.html#post2312906

You could also ask on the Centroid forums too if someone has made a post. Any “Centroid Acorn” post should work, although you may need to remove the tool height cancel G code to make things smoother.

Not “limited” per se but that’s what we officially support.

Why not continue to model in Rhino and just load what you want to machine into VCarve? There are a lot of folks that work that way.

8

Thanks Eric,

I’ll keep working on it,

Cheers,

9

I second Eric’s suggestion of modeling in Rhino and using VCarve for CAM. I was already a Rhino user when I bought my Avid machine. At the time, about six years ago, I looked at RhinoCAM and VCarve. While I really, really (!) liked the idea of having CAM integrated with Rhino after playing around with the free downloads of both RhinoCAM and VCarve, my opinion was that VCarve was much more intuitive and easier to use. Also, at $700, VCarve was much cheaper than RhinoCAM (if I remember correctly, rotary and laser are separate modules that need to be purchased, for example). Anyway, I bought VCarve and have been happy with it. Imporitng .stl objects is easy for 3D carving. The only limit is that in VCarve you can have only one imported component in a file so if you want multiples of something you have to set up the array in Rhino and export as one ‘thing.’ Not a big deal.

Hope this helps,
Garth

10

Thanks Garth,

Solid advice, much appreciated!

Cheers,

11

I’d make a push for using Fusion 360 for your CAM; it is far superior to Vectric, but does have a higher learning curve. You can also do your designs in Fusion too (depending on what you want to make, of course)

Corbin

12

@corbin Strongly agreed - but can’t beat grasshopper!

13

Is the free version of Fusion 360 enough for what folks are generally doing here? If not, it’s subscription based and much more expensive than VCarve Pro.

Also, is Fusion 360 better for CAM than VCarve Pro? I’m asking because since I’m already a Rhino user I don’t really need another 3D CAD package.

Thanks,
Garth

14

vcarve pro costs the same as one year of fusion360. You need the paid fusion360 to support tool changers but the free version will do anything an Avid single-tool machine can support.

In my limited experience, Fusion360’s CAM is pretty good. I tried to stick to FreeCAD (because it’s free and runs on Linux) but switched when its CAM just couldn’t do the complex things I needed, which Fusion could do - correctly - in moments.

15

Thanks all,

Really appreciate the advice. I’ve ended up with F360 and I’m getting some reasonable results. Yes Eric, the switch to the F360 post processor seems to have eliminated my Z axis trouble.

Corbin, I’m looking through some of your YouTube pieces -beautiful work and well explained!

Cheers,

1 Like
16

Following up on the RhinoCAM/EX/Centroid/CNC12 post processors. Is anyone running this configuration? Early on, I was told that there shouldn’t be any issues with that, but now I’m second guessing since there seem to be only two very clear options - Fusion or Vetric - in your postprocessors.

17

We have customers running RhinoCAM.

There should be a Centroid post in there that should be just about what you need. The only thing (from memory) that I recall you have to do is remove the G49 commands at the end of a job run. If you run those you will cancel your Z height offset. It’s not a big deal if you go to run another job, but it can be confusing and potentially cause some head scratching moments when using the touch plate.

Moral of the story is, if you want to use RhinoCAM that’s fine. Post up some G code here and I will take a look

18

Thank you Eric! So grateful for your help.

When I post, I see G49 at the startup. Here’s my code below, unedited with the Centroid post.

When I delete G49 in Line2, I am able to get the tool to touch off (previously, I would get the 907 error before being allowed to run the job). After touchoff, I get the 907 error in Line12, but I don’t see another G49 in the code. Am I missing something?

O001
N10 M25 G49
N12 G17 G40
N14 G20
N16 G80
N18 G90
N20 G98
N22 ;Setup 1
N24 ;2 1/2 Axis Pocketing
N26 T3 M06
N28 G0 X7.662 Y0.621 S20000 M3
N30 G43 Z2.937 H1
N32 M9
N34 G1 Z0.044 F29.3
N36 Z0.019 F14.7
N38 Y0.338 Z-0.031 F11.
N40 Y7.662 F14.7
N42 X7.1
N44 Y0.338
N46 X6.537
N48 Y7.662
N50 X5.975
N52 Y0.338
N54 X5.412
N56 Y7.662
N58 X4.85
N60 Y0.338
N62 X4.287
N64 Y7.662
N66 X3.725
N68 Y0.338
N70 X3.162
N72 Y7.662
N74 X2.6
N76 Y0.338
N78 X2.037
N80 Y7.662
N82 X1.475
N84 Y0.338
N86 X0.912
N88 Y7.662
N90 X0.35
N92 Y0.338
N94 X0.338
N96 Y7.662
N98 X0.382 Z0.013 F11.
N100 Z0.038 F29.3
N102 G0 Z2.937
N104 ;Work Zero
N106 G40
N108 M5
N110 M9
N112 G80
N114 M30

19

I think I got it. Interesting enough, when I post to the “Centroid-IN” as opposed to the “Centroid” post and delete the G49 in Line2, the program seems runs correctly. I’m going to keep testing, but I think I have traction now. Thank you so much for the quick reply @Eric !

20

I believe that’s the only one you need to remove (G49)

You could remove the M9s, (that’s coolant off) but that’s not needed.

If you ever forget to do this and you get to the end of the job and your tool height is cancelled, just start an MTC and the tool height will come right back