Software Hell, or Finding what works for Revolution (Long post!) (Deskproto)

[greecher (Dave)]

My machine is a 1F Elite Masso Journeyman. I first saved my settings to a dedicated usb stick for my normal 3 axis setup before doing anything.
Then I did the setup changes on F1 Screen:
• Setup input 17 to be A-Home Sensor. Note the default was not inverted, so invert it as the other homing sensors are.
• Setup input 23 to be A-Axis Motor Alarm (note my input for this is 10, but works the same)
• Change Homing to include another sequence after Y, ticking the box for A. Note, I double up X & Y homing at same time, so mine was seq3. If separate, then it would be seq4.

Then on the F3 Probe section you will want to update the following values:
• Set X-Offset to -125
• Set Y-Offset to 55
• Set Z-Offset to 35
• Set upper right quadrant to 18/18 as the puck on the rotary for probing isn’t that large, so 18’s will not let it overshoot the y axis.

Now when probing, I probed Z first, then I probed x/y. This will give you the following results:
• Z will be on the centerline of the chuck top to bottom.
• Y will be on the centerline of the chuck front to back.
• X will be +20mm from front face of the chuck jaws. If using the alternate set of jaws instead of the mounting plate, this will give you 25mm of unused stock on the left of the carve.

On the A axis, mine is normally machine zero at -10.9 deg using a magnetic level to check (ie the square stock I have is rotated with the flat spot -10.9 deg toward front of machine). As this would leave the stock for setting up in carving later at an odd starting point, I rotated A to be a flat top, and set A Zero to that point.

I initially tried to use Fusion 360 to set up a model with a bottom jutting cylinder and top cone for clearance, setting up model to use the space from 25 mm from chuck end of the stock to 11 mm to tail stock, or 117mm of usable stock for a 153mm long 2 ¼” square.

Now, fusion 360 has support for a fourth axis, but only if you pay ($$), as it will cost like 10 tokens/day at a cost of $30 for the 10 tokens, bit negative. Also, I had to pull an older postprocessor from blagistein?? that had 4th axis support to get it to work. I was able to use the 14-day trial to get a test, and glad I did, as I did have luck on a smaller test model of rounding the square, roughing it down with a ¼” bit, then using a 1/32” ball nose taper for finishing. It had some errors where the non-cut movements actually intersected prior done sections, but minorly. I then tried the scaled-up version for and that’s where things went wrong, as during the model roughing, it chewed through the model in several places during just movements, and also exceeded the tailstock boundary into the small section with a violent move into the remaining stock, violent enough that the A axis alarmed out, and the carve quit.

pics of mentioned scars from F360 output.

Side note on F360, it will spin the model on a axis like crazy, so I ended up in some cases with the A degrees into the 10’s of thousand degrees. I had to modify the Masso setup to exceed the max A rotation to allow this, an unnatural ungodly act.

I tried very hard to get it to work well in F360, but to be honest, the multi-axis extension is just not really a good fit for the masso/elite setup. It does offer some real 4th axis functionality, and worked wonders on simple operations, but for carving not so much.

At this point I started exploring other options, Vectric, Carveco, and was less than pleased with the Vectrix trial, as $700 for the proper version to do anything, and I was missing some tools I would really like in a software set for a CNC. (note I’m a long time f360 user, and will still continue to use it for 3 axis machining and also model setup for other programs) In addition, Vectric doesn’t really support importing 3d models other than stl’s.

Carveco I shot before I even got out the gate, as it really can’t do much more than column work, not a full bodied stl as a centerpiece, ie wanna do a chess set, forget it, and price again was high.

Lastly I tried DeskProto, and boy glad I did. For only $280 for a perpetual license, you get a well thought out 4th axis experience. It does have the setup for Masso G3 (inch or metric) post processor already built in. I did make some mods to it, as it needs to know more about the 1F setup. On the machine I tweaked the work area, federates, and spindle speeds to match my Journeyman/Spindle. On the Postprocessor, I tweaked the start/end gcode to be more like the official postprocessor output from f360, the spindle speed tab to give correct output (was only originally the S10000 command, not the S10000 M3 command), and the Tool Change tab to add a M9 prior and M8 after call to stop/start the coolant flood ie vacuum.

Some missing niceties, the tools are kind of barebones, ie there is no vacuum use callout, so thus I added it above around tool changes. It also is missing some data, and doesn’t grok like vbits as it requires the shank to be the same size as the major diameter of the tool, something that was a bit wonky, but really no effect on end product.

Now some of the nice, it actually understands square stock! This means I was able to rough directly from square stock down to the model, and only add a finishing pass with the tapered ball nose. In understanding square stock, it will only try to do the milling of the corners first, ie no wasted air carving of the flat faces. It will also maximize model to fill some of that dead corner space. In F360 roughing, I had to tell it how far to step down, ie copypasta several roughing passes to the model because it really didn’t have an effective roughing strategy down to the model rough surface, annoying but doable. In DeskProto, not an issue at all to call out step downs and leaving a skin, it’s callout for roughing above model height, to get the same easy 1 tool affect. I did verify the roughing pass in gcode was doing about .4-degree rotations, as it is by step over size, and not degrees as it was in F360.

Sidenote about inspecting gcode, make sure the first time and anything you change drastically to inspect it, ie your X should not be out of bounds of your workable area, A should stay within 720 degrees, and Z should always be working down from safe height and never really approaching zero (unless you expect it to…). I was able to see that you do get a nice masso preview of the X axis range at bottom, and it clearly shows that my bit would never go below +25 up to +114, my expected work range. It was only after checking my gcode that I caught some of the changes I made to machine/postprocessor/geometry operations that made me confident in the output solution.

Did a sample air carve, and then just ran the job. Success on first try! Deskproto’s gcode breakdown looks very similar in action to a 3d printer, ie if it has separated islands of same depth to do while the A axis rotates, it breaks it into smaller areas, doing each separately, until the two merge again for full length passes, it is very orderly, and the simulations are spot on to actual action. It neatly stayed in its expected work area, never wandering, and gave great results.

Also note the manual/help sections for each sub tab in DeskProto in the setup links to the manual section directly, and the manual does a very good job explaining each item on that subpage.

Last note about object references, I only used the stock probe plate as part of the revolution to get a xyz that sets the center of rotation on A axis, leaving from front face of probe area toward stock, x is 125mm out, y is over the center line also, and z is on centerline of rotation. I didn’t need to probe the stock at all. I like to think in terms of the centerline always, and set the origin of my stock to be the center of that cube. This makes it very repeatable no matter the stock dimensions. I also for my revolution, only change the A0 rotation to make sure the top of the stock was flat to the table using one of them magnetic angle finders. Just measure table on front to back axis, then on top of stock. Mine was built with the chuck Machine A0 actually being -10.9 deg from a flat top. I did notice that once you have probed the revolution, it always is known to the machine for reference x/y/z/a, and so I only had to probe it once no matter how many operations/models I did. Probably only have to do it after machine change over to add revolution back into action.

[greecher (Dave)]

Also, be happy to share the machine, postprocessor & print details. I chose the model as it seemed challenging. Do note that when essentially printing on a “false” 4th axis, some detail is lost, ie there should be more detail inside the veil, and mouth ends should have holes, but as the y axis is basically locked for all operations, it can’t translate out to do that properly.

[OnefinityCNC (Onefinity CNC Official ✅)]

Awesome write up! I think users would like to see how you set up desk proto post processor and settings and such to do the same!

[greecher (Dave)]

Ok, will start working on it,only needed one interested person.

[greecher (Dave)]

Okeydokey, here is what I setup to work for me in DeskProto V8, note if and when you choose your version, make sure you get the multi-axis addition, I also chose the hobbyist license, which is 248 Euro, or the $ equivalent for exchange that day.

test merge.stl (19.8 MB)

I included the model for test purposes, and you can see in the picture I have it orientated along x axis with origin at the bottom middle.

Next up is the Machine Lib. Note I’ll only show the tabs I changed over the default selection. Under Options→Library of Machines you should see this:

It should have your original choice of machine highlighted, I chose the metric version. Just choose Edit. Next up, the main page:

I updated my working area items from defaults, and possibly feedrates. I definitly change spindlespeed and also updated collet to match the ones for my spindle.

Lastly on advanced item, I only updated the correction factor. This gave me over 4 hours 1 min difference between the calculated times and actual.

On to the PostProcesser changes, again choose Option→Library of Postprocessers, you’ll see same as before:

name should be identical to Machine library choice, choose Edit…

I again am only doing tabs I changed, in this case Start/End. Note the spaces at the front of each line. Top of Start Command up to solo G90 pretty stock, M5 is explicit command to turn off laser. End command starts with M9 to turn off vacuum, innocuous to leave in, after that pretty stock moving Z up, A to zero, but I chose to move my spindle back and away from my rotary setup, you can choose differently. Last command does a program stop and rewind. Make sure to add %, as that line won’t get a line#, but if you don’t add it, M30 won’t get a line# as a result.

The Spindlespeed one didn’t have an end command, ie include the M3, so i added it in. This lets the masso controller take over the spindle startup sequence.

Last Postprocessor tab to address is Tool Change. You don’t have to change it if you won’t be running the vacuum at all, but if you do, it first turns off the vacuum, does tool change (manually or ATC), then adds back in vacuum start.

I’ll also add in my part setup, here is my proj list:

small and to the point, first “Geometry operation” i renamed from that generic to Roughing, could have done the same with last which is finishing. Clicking on Roughing, I set it up like so:

I set this up to use my Masso ATC cutters in the Library of Cutters, choosing a straight cutter adn feedrate and spindlespeed. Note, I chose too fine of a distance between paths, it could have been rougher than that, say 1.5mm.

Strategy tab:

I chose the simple parallel along X axis. The Main looks interesting choices, but I’d keep the details the same. The manual does a excellent job of explaining the choices, simple hit the help button. Next up Roughing tab:

Under Layers, sub section, I chose custom 3mm. This sets the depth of cut for each roughing pass down to the remaining skin depth you choose. .5 or 1mm should do fine to leave most of the finishing done by the ball nose bit. I didn’t originally chose the ramping angle, but noticed that it will just plunge down your depth of cut to just start the pass, so I’ll be doing future with the ram set.

On the finishing step, general tab, updating cutter, precision, feedrate & spindlespeed. The

On Strategy, I again chose same as roughing, parallel along x axis. On Roughing, it was no layers use, and zero skin thickness.

Just to quickly cover a cutter setup here is for my 1/4” downcut bit:

Important things to know for ATC is tool number, probably free length (the length extended beyond the spindle nut, and cutting length.

Lastly, I didn’t cover this first, to start a new project similar to mine, you would choose as below:

After that you can double click the Part to get the Part Paramaters, it is the second item in this list:

You’ll see this screen with tabs:

make sure to check use rotation axis, as this tells the software your going to do a rotary.

On the transform tab:

you can play with the rotation to get your mid axis to be down the center of your part, make sure center geometry is checked.

The material tab has this stuff:

with the important part being the shape. I chose Rectangular centered, but if you have a cylinder or possibly eccentric, you can take advantage of that.

I don’t think I changed the zero point tab, but here is what it is:

lastly, an alternate way to get to part parameters is this (right click for pop down menu):

This is where you can add more geometry operations, ie more toolpaths.

Note this software I only covered as to 4th axis, it is actually a fully formed 3 axis tool also, but I like to do my design work in 360, but it looks like you could for a cheaper set price make this work all the way around. As for BB installs, I think this would work better than just fine also. Check out the vector ops in particular, seems to be deep in that regard also for vcarving or just plain dxf cutouts. Do note on the part parameters page, it’s a simple uncheck box for use rotation axis, so the multi-axis software supports both 4/3 axis normally.

If you are looking for a good alternative software for either rotary or just 3 axis, this for my first cut is just good. Note I only found out about it yesterday afternoon, purchased it from the developer just last night after more research, and installed, configure, and ran my first project this morning, it is stunningly good for affordable software that is a decade old! the website is not up to date, but V8 is out within the last year, and documentation and tutorials have also been updated.

Cheers,

Dave

[PezWoodworks (Pat)]

Wow what a lot of effort for the group, thanks for doing all this, not many will go to this degree of detail to help out.

Thanks,

Pat

[greecher (Dave)]

As I kind of struggled to get rotary to work, thought I would put out some of my thoughts and where things kind of went sideways etc. I saw quite a few questions about how, so hopefully this will help others.

[rdjennin]

Fantastic write up and explanations. Very much appreciated.
Does anyone know which post processor in Deskproto to use for the BuildBotics controller?

I can seem to find one.

[greecher (Dave)]

rdjennin,

the process of doing up your own post processor isn’t too frightening, as I just looked over all of the tabs, and it isn’t as intense as writing up a .cps file or something. You can take the one I suggest (masso in or mm), copy it to a new one, rename name/file, and checkout the different tabs. The customizations I did are probably similarly desired. I’d double check the output of the newer pp, and tweak as desired. Do an air carve for first runs.

[rdjennin]

Excellent, thanks for the advice. Much appreciated.