5-axis with RhinoCAM

We have a 5-axis Shopbot at Assentworks, bought it with the RhinoCAM software shopbot bundles with it. Are there any other 5-axis users out there?
I have tried to search the forum for threads about this, but can't find anything.

We have had the machine for several months now, and the machine itself is up and running (ie I can run it through its motions using the Shopbot control software). I also managed to set up Rhino and RhinoCAM, and to post some code. I am stuck, though at getting Rhino to spit out code to move the a/b axes.

The version of RhinoCAM that is shipped by ShopBot with the 5-axis do 5-axis paths by first setting a reference xyz system (usually other than the regular xyz) and then doing a 3-axis tool path against that. When I post this and run it in ShopBot3, the x/y/z axis appear to be travelling the way they should, but the a/b axis "wrist" doesn't rotate. I suspect I am missing something quite small, but it has me stumped.

Have any of you worked with this?

Can you post maybe the first 100 lines of the .SBP code that RhinoCAM puts out?

Also, when you are in SB3, do you see the A & B axes enabled (with some numerical value) on the Red DRO screen? If not, run the VD command and set number of axes to 5.

There are not many 5-axis users that frequent this forum. You should contact SB Support to make sure you have the right post processor and configuration for your tool.

-B

Can you make sure the 5 axis machine tool is defined correctly under the Machine Setup dialog in RhinoCAM. Set the number of axis to 5 axis, Configuration to Head-Head, Primary axis as Z and secondary as Y axis.

If you are still unable to get the primary & the secondary axis output on posting processing the machining job or the setups, please send us the programmed part file (*.3dm), the posted output file (*.sbp) and a copy of the 5 axis post processor you are currently using (*.spm) to support@mecsoft.com so we could take a look at it.

MecSoft Support
18019, Sky Park Circle, Ste KL
Irvine, CA - 92614
(949)-654-8163
(949)-654-8164 (Fax)
www.mecsoft.com
support@mecsoft.com

Quote:

---

Originally Posted by bradywatson

Can you post maybe the first 100 lines of the .SBP code that RhinoCAM puts out?

---

Here are the first few lines. I looked further, it never does seem to get into additional parameters:
JZ, 0.0000
J2, 0.0000 , 0.0000
M5,,,,0,0
SO,1,1
'Horizontal Roughing
J3,-6.0472,-4.2878,-2.3776
MS,0.2,0.2
M3,-5.8357,-4.1264,-2.6764
MS,0.1,0.1
M3,-5.8225,-4.1164,-2.6950
M3,-5.8066,-4.2334,-2.7809
M3,-5.6790,-4.2252,-2.7192
M3,-5.7966,-4.0734,-2.7204
M3,-5.7935,-4.2234,-2.7993
M3,-5.6790,-4.2252,-2.7192
M3,-5.6513,-4.3396,-2.7614
M3,-5.8230,-4.3369,-2.8814
M3,-5.8547,-4.3241,-2.8970

Quote:

---

Originally Posted by bradywatson

Also, when you are in SB3, do you see the A & B axes enabled (with some numerical value) on the Red DRO screen.

---

I see them and am able to move them with the program. Also am able to do the zeroing routine that does include them. I am reasonably sure this is not a controller issue.

Quote:

---

Originally Posted by bradywatson

There are not many 5-axis users that frequent this forum. You should contact SB Support to make sure you have the right post processor and configuration for your tool.

---

I figured there were not many, but thought I'd start the conversation to see what is out there. The RhinoCAM people posted in the next post, so that will be promising!

Good to see MecSoft helping.

FYI:

This is the only 5 axis move I see, which only moves A & B to 0 on each axis.
M5,,,,0,0

This is a 3-axis move, where only X,Y,Z moves are present.
M3,-5.8357,-4.1264,-2.6764

M5 commands would have moves for all 5 axes, although depending on what you are doing, there may only be values for a few of the axes. For instance, this would be a valid move:

M5,-5.8357,-4.1264,-2.6764,,1 (X,Y,Z,A,B) - no movement change on A

You won't get any movement on A or B unless you have both an M5 command and a parameter for both A & B in the 4th & 5th spot respectively.

-B

Matthew- note that the snippet of code you posted marks the code as "'Horizontal Roughing". Logically that would only be 3 axis machining, even if the post processor will later insert the 5 axis machining instructions.

The roughing pass is designed to get a lot of material out of the way quickly and easily. That means "easy to compute" for the tool-path generator also. 3 axis code is much easier to generate than 5 axis code.

Look for 5 axis motion much later in the file. It should still be a lot of lines of code. There is not much simplification possible for 5 axis move commands.

Feel free to skip the following "off topic" 5 axis toolpathing issues.

5 axis toolpathing is done with one of several strategies, one of the simplest is to keep the bit perpendicular to the final surface. That requires a lot of math to compute for each point that needs to be machined. The good part of this method is there is only one place where the spindle can be and have the bit perpendicular to the final surface. It also positions the cutting axis in places that may "collide" with not-yet-removed material. The spindle location needs to be checked for collisions also. That is another job of the roughing pass, remove the material to prevent these collisions during 5 axis surface milling.

Another strategy is "tangent" milling, which is can be even stranger to compute than "perpendicular" strategy, because the bit can lay across the surface in any of 360 directions. Which one of those directions keeps the spindle out of the way? Which is the fastest and easiest to reach? Does it prevent gouging of other parts of the surface?

Collision avoidance is one of the nastiest parts of designing a 5 axis toolpath generator.

I have never worked with Rhino beyond the demo. But generating toolpaths for 4 and 5 axes is something I have worked on.

Thanks MecSOFT, I have sent you an email with the files and settings currently used.

Dana, when we originally received RhinoCAM I was quite frustrated because the version Shopbot bundled with our machine (ie specifically for a 5-axis robot) does not include full 5-axis machining. Aparrently there are different grades of RhinoCAM, and the true 5-axis one is quite a bit more expensive. it would be able to do the perpendicular tool path you describe, no idea how good its collision avoidance is in the process
.
After messing with it for quite a while I asked ShopBot how the limited RhinoCAM is supposed to work and they explained that I would need basically use 3-axis cuts after setting a reference coordinate system different from the normal one. For example, I might cut something by first creating a toolpath that treats the object's right side as "up", and then a second one that treats the left as up. Depending on the shape and my choice of reference coordinates systems, I might be able to get the job done in two toolpaths.
So, when you saw "horizontal roughing" in the code, it was indeed a 3-axis path, but tilted into a different coordinate system. From what I saw in my testing with the Shopbot, the x/y/z movements actually look about right, but that is no good unless the a/b rotates to the new "down".

Using this 3+2 approach I suspect collision avoidance becomes _almost_ as simple as for regular 3-axis machining, except for the z-pillar.

I feel a bit ripped off by this choice of bundling, but I guess you get what you pay for, and to stay competitive Shopbot decided to only include the very minimum need to make it work.

We have sent a response to your email on Friday, Sept 27 2013 and would like to follow up to make sure you have received it.

MecSoft Support
18019, Sky Park Circle, Ste KL
Irvine, CA - 92614
(949)-654-8163
(949)-654-8164 (Fax)
www.mecsoft.com
support@mecsoft.com

I am switching to this ID from the one I borrowed from our main Assentworks Shopbot guy before.
Yes MecSoft Support MecSoftSupport, I got your email, thanks. Just only get to the ShopBot once a week.

MecSoft's suggestion was: "To output the a and b angles (primary and secondary axis angles), select the setup folder "whacky angle", right mouse button click on it and select Post."
I had right-clicked the tool path inside the setup in the past, so tried this, and sure enough, I now get a 5-axis move:
M5,,,,217.35,41.67

I have not yet had a chance to actually run this code, but this is a lot more promising than before. I will post where this gets me when I have a chance to actually test. Thanks MecSoft!