V Carve Scolloping, how to prevent

[Peter Rawlings]

I've attached photos of something I'd like to eliminate, but not sure what to do. Thought I'd pick the brains here before experimenting with feeds and speeds to hopefully find solution.

These are 8x8" "tiles". Ranger high density MDF, Cutting on Shop Sabre 408, 10hp spindle. Using Amana 120°, 2" dia. double insert V cutter. 18,000 RPM, feed 180 ipm, plunge 30 ipm. Vacuum hold down.

Some of the facets are smoother than adjacent, I imagine something to do with direction of travel and rotation. Barely noticeable when cutting, but can see and feel upon closer inspection. Photos shot with a sealer coat.

What say the brain trust?

P1070213.jpg

P1070222.jpg

P1070237.jpg

[David Falkner]

Are you doing a rough cut and finish cut? I would climb cut first and take a full depth conventional cut final pass, say 0.004", to finish and see how that does. I know that adds to the job time but if it shortens any finishing steps or makes a better end product then you're ahead of the game.

David

[Peter Rawlings]

I hadn't thought of that, David. The way this cuts with a v-carving toolpath, it plunges the vortex of triangle and then slopes out to the points. Is there a way to change cut direction in v carve or should I be using a different toolpath? I imagine I could do final pass by setting up z-zero a few thou high. I'm not given the same options as a pocketing toolpath. Is this a difference between Aspire and V Carve Pro?

[David Falkner]

Can't answer that, Peter. I use Fusion 360 and in almost every profile I can choose whether I want the cut to be climb or conventional, which was my basis for the question. I'm sure some of the Vectric users will chime in soon, but like you said, you can change your Z height by a couple of thousandths and see what that does.

David

[Bill George]

I do not think in the V Carve mode there are choices on direction of cut, It might be a feed speed or Rpm issue. But no rough or finishing.

[Jim Becker]

I think that "Chatter" is from something physical, either related to speed/feed or, perhaps, something in the gantry isn't secure. Check for the obvious stuff in that respect. I had a small issue with quality of cut/accuracy with my CNC when I first took delivery and was finally able to trace it to something not being tensioned properly at the factory or knocked out of tension during transport. I've never got that kind of chatter with a v-bit, but have seen variations of that early on with straight cutters before I got serious about checking everything.

You may also be taking "too big of a bite" for the material, bit and speed/feed.

[Mark Bolton]

My guess is the feed is too aggressive for the 2z cutter and depth of pass. I would try adjusting your feed, depth of pass and clearance pass stepovers, or setting up a final skim toolpath as Peter mentions.

[Jerome Stanek]

I would try running it in the opposite direction

[Martin Wasner]

I don't think you'll gain anything doing a climb cut in mdf.

My guess is to reduce depth of cut and do a final pass at depth.

If that doesn't take care of it, then something is off.

I'd inspect the spindle and make sure it's grabbing the tool holder correctly. Also check the seat for any debris. You're not supposed to blow air up in there, just wipe it with a rag.

I'd give everything on the gantry and give it a rattle and see if something is loose.
Do you have a torque wrench for tightening the tool holder?

How good is your dust collection? Do you have blowers moving chips out of the cut?

[Brady Watson]

Try cutting a sample piece, one quatrofoil (4 triangle set) at 60,60 IPM @ 18k RPM. See if this improves the quality. If it does, increase XY speed only until the chatter shows up again. Then back it off.

You may also want to cut another sample at a lower pass depth, giving you less material to take off on the final pass. Keep in mind with v-carving that the deeper you go, the volume of material increases exponentially.

I am seeing some signs of possible reverberation in the corners on some of those pieces. Keep in mind that it isn't possible to actually go 180IPM (3 inches per second) on a cut that only traverses the part say 2.5"...It'll never get there and this sometimes results in jerky movements while the controller does its best to achieve the set speeds.

[Peter Rawlings]

Thanks for the insights. I'll catch y'all up on progress.

I'm recent to the game of CNC. My only real-world software familiarity is with V-Carve Pro which decides much of how the spindle will move when choosing the "V Carve" toolpathing. This limits what one can choose in the way of cutting direction which would be available in a different toolpathing option, such as pocket or profile. I suppose it would be possible to cut this as a 3D model, but with a way-too-long process time. While dust collection is good by my standard, I don't currently have ability to shoot a stream of air at cutter...an interesting idea I'd like to hear more about.

I've troubleshot in many of the ways suggested. Spindle speed up to 20,000 and down to 15,000. Movement by increments down to (way slow) 20ipm. Shaken, yanked on, inspected, greased, all I could think of on gantry. Narrower angle V cutter, different tool holder. I suspect the problem is magnified by the shallow angle cutter. I don't really think this is what I term as chatter, which would be more like material hold down problem or spindle/ cutter run-out issues. Perhaps that's my distinction only. It might also be somewhat material related. When I get a chance, I'll run test battery on solid surface material and see where that takes me.

I tried to methodically leave no stone unturned. I was able to reduce size of scalloping cutting in a single pass significantly by slowing down below 60ipm. Near perfect at 20 ipm, but I imagine the cutter churning away in a flurry of MDF swarf, maybe even burnishing the surface. Besides that, it's just too slow for the production I envision. Good surface finish was also achieved by a .005 final pass. Downside is that doubles machining time which shoots foot of production.

On the horn with ShopSabre we discovered a slight, I'm guessing .003-4, in Z ball screw endplay. Shims to bring that closer to 0 on the way. I'll update once installed and tested.

Thanks again for the help with my big toy!

[Brady Watson]

I'm guessing .003-4, in Z ball screw endplay. Shims to bring that closer to 0 on the way. I'll update once installed and tested.

That makes sense. The bit, with any significant cutting force against it, is wandering in that hysteresis/backlash along the cut. At high RPM & low feed rate (aka low chipload) there isn't enough cutting force being exerted for the marks to show up. In case you haven't held a spinning router in your hand and spun it around a little - the CNC is essentially controlling a gyroscope. Any slop/slack etc in the mechanicals on the machine will allow it to wander...and those chatter marks point to exactly that.

Glad you tracked it down and have shims on the way.

FYI - rather than 'guess' at something you can't see, a $25 dial indicator can show you exactly how much backlash you have in each axis...It is one of the most useful measuring devices in the shop, regardless of what machines you use.

[Peter Rawlings]

FYI - rather than 'guess' at something you can't see, a $25 dial indicator can show you exactly how much backlash you have in each axis...It is one of the most useful measuring devices in the shop, regardless of what machines you use.

That was my hip shot using 63 year old eyeballs along with built in feeler gauge (hand). Will measure with indicator when I disassemble so I can get a straight shot down on to ballscrew shaft...drive motor in the way. Unwilling to do that until shims in hand as it's still functional as is, just not for this particular task.

Yep, know that gyroscopic effect well. Handheld router fetish long before CNC came my way. 15 or 20 all told, I imagine, but that may be TMI about me...

[Gerry Grzadzinski]

That's definitely a mechanical issue.
I recently used that same Amana bit (RC-1104?) to make some large maple raised panels on our Morbidelli, and all the cuts were glass smooth.

[Martin Wasner]

We use the big 91º one for miter folds. Similar results to Gerry, super smooth cut.

Mdf is going to be the easiest of materials to cut.