forum.cncdrive.com

Good evening to all,

My name is Laurent, I'm based in France. I've started some months ago the building of a rather large (3500 x 2000 x 1300 mm) gantry type mill, in order to (someday...) machine 3D master forms used to create molds. Materials will be foam, wood, maybe some aluminum if the machine is rigid/strong enough.
My plan is to start the machine using only X/Y/Z axis, with a slave axis for the 2nd X axis motor. If everything is OK on the machine structure and geometry, I will then add 2 rotary axis to the spindle head.

As I'm making progress on the build, I'm trying to educate myself on the intricacies of CNC controllers and choose a suitable solution for my project. It seems that UCCNC would be a good candidate, so I downloaded the software, run it as demo for a while with an eye on the documentation (very good job on this by the way ). I think I have understood some/most of what I've read so far, and I like what I saw, but I have a few questions :

- Is it correct to say that all axis are treated by UCCNC as linear axis ?
(I could not find a way to specify a rotational axis in the axis settings, and another discussion on this forum seemed to say just this)
- when using an axis as a rotational axis, the Unit used to define the speeds, limits... is actually a degree (or radian ?) rather than inch or mm ?
- is this possible to interpolate on linear and rotational axis simultaneously ?
- how does this impact the GCode ? Is it possible to get a 3D capable CAM software to post to UCCNC directly ?

I still don't know for sure which CAM I will use. At the moment, I'm using Fusion 360 for the design of the machine, and I know that this offers 3+2 axis at the moment. Anyone using this with UCCNC ?

Thank you for your help

UCCNC does not use rotational axis.

As a work-around, I have set my 4th axis (along-X) to have steps per unit as a fraction of 360 degrees. I'm using Fusion360, and the post processor outputs in degrees, which UCCNC interprets properly when the steps/unit and stepper driver settings are adjusted appropriately.

I believe that CNC Drive will be adding support for rotary axis, but it'll probably be a year or two away.

Thank you for your replies.

spumco wrote:UCCNC does not use rotational axis.
As a work-around, I have set my 4th axis (along-X) to have steps per unit as a fraction of 360 degrees. I'm using Fusion360, and the post processor outputs in degrees, which UCCNC interprets properly when the steps/unit and stepper driver settings are adjusted appropriately.

OK. I think that I understand, but I'm not 100% sure I can see that by using appropriate settings, you can get UCCNC to generate the correct move to tilt your 4th axis according to the value asked for by Fusion360. Then where is the limitation/difference with a 'proper' rotational axis ? (coordinated motion, feed rate calculation, tool length compensation, other ?)
Could you give an example of GCode block that includes a 'rotation' of the 4th axis and describe what happens on the machine when the move is executed ?

ger21 wrote:I believe that CNC Drive will be adding support for rotary axis, but it'll probably be a year or two away.

I've seen that there is a feature request that has been posted, good to know it is being considered. I guess that if this requires such long time, that's probably because there is a lot of work involved, much more so that my current naive understanding can imagine.
On the other hand, seeing how 'fast' I'm making progress on my build, this might become available just in time for me

It all depends what you want from the rotational axis and how you are going to use it?

Are you going to index its motion (do a cut at one positon, move the rotational axis, do another cut, move the rotational axis etc...) {easier to do + you can hack it now via macro}

Or are you looking for blended axis motion (rotational axis moving at the same time as the linear axis + compensating spindle speed / feedrate) {much more difficult to integrate}

I plan to add 2 rotational axis to the spindle mount, so as to be able to tilt the spindle and reach points that could not be machined with a fixed, vertical tool (e.g the bottom of a high vertical 'wall'). I will probably start in 3+2 axis mode, where the cutting will be segmented, and the head orientated between segments like what you describe. You mention the use of a macro to do this, can you give a rough idea of how this could work ?

It would be nice to be able later on to 'upgrade' to blended axis motion, but I realize that this is much more difficult, starting with a CAM package that will be expensive and possibly difficult to learn. At the moment, I'm trying to understand what the current version of UCCNC would allow or not, so that I can make an informed decision.

Thank you for sharing your knowledge

I just noticed that your signature includes a link to UCCNC Macros doc, I'll look into it to get a better understanding of the subject

Full 5 axis is a whole different ballgame.

What I was referring to was rotary 4th axis. I wouldn't think that CNC Drive will be adding 5 axis support any time in the near future, as it's an incredible amount of work for a handful of users at most.

In 15 years of following DIY CNC forums, I've probably seen less than ten DIY 5 axis machines.
I believe that 5 axis requires the control to support some type of kinematics, to keep the tool in the right position/orientation.

ger21 wrote:Full 5 axis is a whole different ballgame...

Agreed. I don't want to sound brash and make unsubstantiated/arrogant claims, I'm just trying to understand the lay of the land here
And I have a lot of reading to do before I can stop asking stupid questions, so thank you for your patience !

My 'workaround' works for indexing only. Fusion output example:

G54 G90
G0A90
(4th axis will rotate positive 90 degrees)

As long as you set your steps per unit so that 360 units = 360 degrees of rotation, UCCNC and Fusion play well together. With my 4th axis worm-drive ratio, and my steppers set at 10x microstepping, 500 steps per unit = 1 degree of rotation. I can usually get the table or vise flat across Y to within 0.0002"-0.0003" by jogging in 0.01 step-units.

I haven't tried backlash comp on the 4th axis yet - I have about 0.08 degrees of backlash - but I could hand-edit the Fusion code to move only in one direction, or to move past the desired angle and then back (just like manual machining with sloppy lead screws).

As UCCNC doesn't have diameter compensation, it will not work for 4th axis continuous unless the OD (or tool path) doesn't change in distance from rotational axis.

At least, this is what i think. I haven't tried it yet, but will probably put some nylon in the 4th chuck just to see what happens fairly soon. My guess is that the feed rate wouldn't be all that appropriate if the Z or Y distance from center-line is continuously moved during cutting.

As for Fusion 360, it's critical to consider the rotational axis during the modeling and CAM phases. Assuming A rotates around X, then the work origin needs to have the Z & Y on the center-line of your rotational axis. In my case, I modeled my 4th axis and trunnion table (and adjusted to 'as-built') and import them in to the Fusion component. I also added a construction axis that is on the center of rotation, along with a model of the stock I'm using.

Once they're imported, the vise, fixture, or whatever is assembled to the trunnion table and a point is created along the rotational axis and at the edge of the stock model. Moving over to CAM, I set the work origin at the point created earlier, and then during the various operations I change the tool orientation to the desired angle. Fusion outputs the A-axis indexing properly.

Tool touch-off is accomplished by using a wiggler to find Y0 (dowel pin sticking out from and along rotational center-line), and Z0 is set with a 1-2-3 block on the table surface (plus a bit - my rotational axis centerline is 2.2085" above table). X0 is set at the edge of the stock.

Seems to work for me so far, but as usual I'm extremely new at this so you may find a more efficient workflow from someone else.

5th axis continuous - I can see trying this in the future, using a rotary 5th table and not a moving mill head. SkyfireCNC has recently come out with a harmonic drive 4th/5th axis device, and I suspect it's reasonably inexpensive compared to big-name stuff. I have a few (paying) parts whirling around in my brain that would be perfect for 5-axis work (even if it's just 3+2 indexing).

-Spumco