ShopBot Circles cuts out of alignment

[CDarby67]

Hello,
I had some issues over the weekend while using a maker space ShopBot. I am cutting Polycarbonate 0.375' with a 1/4" single flute "O" up cut - Onsrud. (I have cut the same part with the same bit in, on a Laguana with no issues).

Speed 18,000 IPM 60, depth of pass 0.100" 4 passes. The center hole is not circular and the tabs cause a gouge in the periphery circle.

Suggestions?
Thanks,
Clint

[EricSchimel]

Looks like something is loose on that machine.

Try this:

Power it up and make sure the steppers are locked. Pull and push the gantry on the X axis and check for any play. Do the same for Y.

If it's a V roller machine (the larger format SBs) you can put your finger right on the V roller where it lands on the track and when you push and pull you can easily feel for any play.

For the Z axis flip a bit over and chuck it in the spindle/router so the smooth side is sticking out. Grab onto the bit and see if theres any wiggle to it.

If you feel any kind of play anywhere get out a dial indicator and start diagnosing further.

[CDarby67]

Eric,
I will try those recommendations. My thought was that the machine is WAY out of calibration. It is a public maker space. Additionally, the maker space takes commissions from the community and they recently made a few thousand face shields - as you can see the waster board was trashed. Ultimately, I can not do any calibrations - it is not my machine. I will however recommend they have it serviced. They had new waster boards on a cart waiting for install and surfacing.
Thanks,
Clint

[coryatjohn]

Your cuts are pretty aggressive. 0.1" per pass on polycarbonate takes a lot of power to do. I suggest trying a much lighter touch and cut half the depth per cut (0.05") at half the speed. It's the cutting force that really brings out the slop in a machine. The cut quality will improve too.

Another thing you can try is to leave an offset on the part and either sand it off or use a final pass (or another cut file) to trim the part to final size. The lighter the touch, the better the cut, especially with a worn out machine.

[EricSchimel]

Clint, what type of machine are we talking about? PRT, PRS, PRS Alhpa? Desktop? DesktopMax?

Cory, even on a PRS Standard, those speeds and feeds sound slow. Polycarbonate cuts like butter but can melt at slower speeds. If it were a PRS Standard I'd do 2.5 IPS, .25" depth per pass (with a .25" bit). If it were an Alpha .35 per pass at 4-5 IPS would do well (16-18k RPM)

Clint, if you were cutting too aggressively and you lost steps you'd see shifted circles, not oblong ones like you've got there. That machine, whatever version it is has something loose on it. You've got to figure out what part is loose. While it's up to the maker space to fix it, depending on what it is it might be very simple to do a field repair.

[CDarby67]

Cory - thanks. I used same bit/feed/speeds on the Laguna (Open Works Baltimore) and it cut perfectly.

Eric - PRS Alpha.
My first run of the same part I used the 0.25 cut per path - my initial thought was I was hogging too much with each pass. I run 18k per Onsrud recommendations.

This machine is used by the public with minimal experience and no vested interest in keeping the table running well. I sent an email to the management requesting a calibration and PM.

While I have your attention (greatly appreciated), How does ramping effect the simple parts I am cutting? I know it is easier on the bit - correct?

thanks
Clint

[srwtlc]

Grab the nose of the spindle and give it a push/pull in the long axis and feel for play in the lower v-bearings of the Y car. There should be no play in it. Check for play due to the motors/pinions not being adjusted into the racks properly.

Use 3D tabs and match your plunge rate to the feedrate, this will allow the tool to flow through the tab sections instead of dwell/up/move/dwell/down/dwell/move....

One other thing, are you using an arcs-inch post?

[CDarby67]

SRWTIC - I am unfamiliar with what you mean regarding Arcs-inch post? I am new to CNC, this forum, and ShopBot. I had seen 3d tabs and looked into them. I will try it with my next layout. I had the tabs set to 0.0625' and had them placed at 2,5,8,11 as if on a clock face. setting the plunge rate to the feed rate makes perfect sense - I will do that.

Eric - I did not see the recommendation to do a field repair - is there a YouTube video I can look at? I am (at this point) 100% convinced that the machine is loose because of abuse, use, and lack of PM.

Thanks,
Clint

[srwtlc]

Assuming that you were using a Vectric product, when you choose a post processor to save a toolpath, one of the posts in the list used to be named ShopBot_inch (or something similar) and that one would only output segments for circles/arcs, which can cause poor quality circles. There's a arc_inch one or the Shopbot_TC inch/mm ones that output arcs instead of segmented arcs.

The deal with 3D tabs is that they run along without the dwell or stop and start on the tab, which is in part causing the divot on your tabs. If the plunge rate is less than the feedrate, you can get some of the same thing happening, but by matching them, it keeps the motion going with little to no dwell at the tab. Keep in mind, the actual tab length will be minus the tool diameter.

[EricSchimel]

Hey Clint, I hesitate to recommend a field repair until we/you figure out exactly what's going on.

My guess is the the V rollers are loose (easy fix with a wrench and an allen key) if the pinions are worn that's also an easy fix, although you would need replacement pinions.

Everything else Scott said is on point. Here's some elaboration in no particular order:

Ramping in can in some cases remove "witness marks". Basically those are small marks where you can see the tool entering and exiting the material. These, if they exist should be superficial. What you've got it something that's mechanically out of whack however so a post won't solve that 100%

As far as the "TC Arcs" post processor...

There are a couple of ways a post processor can cut an arc: The wrong way or the right way.

The wrong way is when an arc is treated as a bunch of little tiny line segments. That's not an arc. An "arcs" post processor will actually tell the ShopBot "Hey, this is a circle do do one of those" and the SB3 control would automatically smoothly more around a circle.

Using the wrong post won't cause the issues you're seeing, but for circular/arc'd stuff you definitely want to add that to your checklist for getting this machine sorted.

[coryatjohn]

>> even on a PRS Standard, those speeds and feeds sound slow.

Sounds like the machine is worn out. Slowing things down reduces the forces on the end mill and should reduce backlash in the system. Cutting both the depth of cut and speed by half should yield about the same chip load and reduce the forces acting on the machine by a factor of four. Naturally, adjust the RPM's to compensate and get the best cut quality.

[EricSchimel]

But that doesn't suss out or fix the problem. A loose or out of calibration machine should be fixed now matter what speed you're cutting at :)

[coryatjohn]

But that doesn't suss out or fix the problem. A loose or out of calibration machine should be fixed now matter what speed you're cutting at :)

I totally agree except that in this case, the OP doesn't control the machine. So if he wants to use it, he'll have to work around the limitations of the equipment. Of course, if he can get the workshop to fix it, that would be great too. How long will that take?

[EricSchimel]

Knowing what's wrong with it will determine whether or not there's even a work-around that works. Also, being in a shared workspace it'd be nice to be able to tell others/those in charge of fixing it what might be wrong with it.

Blindly dropping feeds and speeds is a crapshoot at best for getting accurate cuts on a compromised machine.

[coryatjohn]

Ok, if you want to argue, that's great. I'm finished with my thoughts on the subject.

Have a nice day!

[EricSchimel]

Sorry you took that the wrong way... I wasn't trying to argue, I was just trying to help solve a problem.

My thoughts simply were that if you can pinpoint the problem you'll learn a lot, and either be able to fix it or do a proper workaround if that's needed.

Again, I wasn't trying to argue with you at all, I apologize if you took it that way.