Many Small Circles in MDF

[kevbo]

I've been attempting to cut dozens of 1.1" circles through 3/4" mdf with a 1/2" x 1-5/8" carbide upcut spiral bit.

First attempt - results poor. circle was hardly that.
I searched through the forum and found some ideas on changing ramp settings and I'm 'getting there'.
Problem I'm finding, the circles are slightly out of round - consistently. I've tried various speeds and feed rates but with the MDF, I worry that going too slow will cause the bit to heat up.
I've tried half depth cuts and full depth cuts and the quality of the hole really doesn't change (by adjusting the move speed accordingly)

Does anyone have any suggestions as to router RPM / feed rates or ramp settings to cut these circles out? It is the porter cable router router - not a a spindle, on a PRT Alpha. (48x96 bed)
Also - on a hunch, I tried doing some measured rectangles and I'm finding that the shopbot is cutting longer than it should be (by 1/16" or so) in the X axis which I feel could be a problem as well.

[harryball]

1.1" or 1' 1" ?

Dang... if it's 1.1" with a 1/2" bit upcut... well there's your problem.

I'm going to assume the 1' 1" for a moment. First, try a compression bit and using a spiral toolpath. For me that has worked well.

Do the basic stuff, check the square on the gantry and that your Z axis is square. It is very normal as a router travels in a circle to get torque forces flexing the gantry as it moves. One way of coping is to cut your circle oversized about 1/32" or even 1/16" and leave an onion skin on the bottom. You can cut fairly aggressively. Then make a gingerly full depth cut to the correct size. Don't be afraid to try both conventional and climb directions.

Good luck!

/RB

[jerry_stanek]

I see he said small circles so I would assume 1.1

[srwtlc]

Check for machine slop in the form of loose pinion gears. Tighten up if needed.

Check for square. Measure that rectangle from point to point diagonally. If it's skewed, your not square.

Check for distance moved. If you move 12" it shouldn't move 12.0625". Use a gauge block clamped up against some place that you can move the gantry and check that it is moving the commanded amount from say 0.0 to 6.0 and so on. If it doesn't, verify that you have the proper unit values (VU) for your machine. X and Y value should match.

What post processor are you using? You should use one that has "arcs_inch" in its name. If you use one that just has "inch", your arcs/circles will be segmented moves and can cause poor cuts.

You shouldn't get much if any bit deflection with a 0.5" bit, but if you move too fast, you could get some machine flex. Again, check for machine slop with the motors locked in.

How tight is your PC router? Runout?

Hog the hole and then follow up with a lighter/slower pass to clean it up.

Scott

[knight_toolworks]

a .5 bit is pretty large for 3/4" material. try a 1/4" bit. try a 1/4" downcut and the parts will stay in place on their own.

[feinddj]

Although it will add to you time, try a spiral ramp and use a down cut. the spiral ramp will clear the chips and not put to much stress on the part.

[kevbo]

The dimensions were correct a 1.1" diameter circular holes. I typically use the shopbot for large scale / large pieces and I guess it never dawned on me that a 1/2" diameter bit should not be used to cut 1.1" holes? Is that due to the 'resolution' if you will? In essence, because the bit is essentially half the hole, it would have to move in a perfect circular motion which is asking too much with the type of forces / gantry movements involved here?

I thought it would be best to use a larger bit to clear the entire hole out, and not leave any loose tiny pucks, but perhaps that was my mistake in the first place.

Is the spiral ramp cut setup as part of the toolpath? I couldn't find that in the interface anywhere but I will search the forum for it.

I will check the machine for square again. Honestly, up until now, our parts needed only a +/- 1/8" tolerance and I noticed in the past that it seemed to cut 'longer' than it should in one direction.

The xy values are the same and I have never changed or touched them.

For my testing purposes with these holes, I was creating them in Parts Wizard and exporting them directly to the shopbot - they were not segmented but beziers and arch_inch was there as I saw it.

Thanks for all the comments and suggestions - I will try a smaller bit as perhaps that is where I went wrong in the first place.

[srwtlc]

If things are running right, I don't see (haven't seen) where the 0.5" bit would bother with exception that you're using a router instead of a spindle. My choice of bit would actually be a 0.375" compression. It's a good balance of size, strength, and power required to spin. A downcut is going to cause more heat and a 0.25" one is going to deflect some. I don't think PW has the spiral ramp that VCP and Aspire have. With a pocket or profile cut and a 0.375" bit, the waste would be small enough that it will get sucked up the dust hose.

Scott

[jim_ludi]

Check for machine slop in the form of loose pinion gears. Tighten up if needed.

Check for square. Measure that rectangle from point to point diagonally. If it's skewed, your not square.

Check for distance moved. If you move 12" it shouldn't move 12.0625". Use a gauge block clamped up against some place that you can move the gantry and check that it is moving the commanded amount from say 0.0 to 6.0 and so on. If it doesn't, verify that you have the proper unit values (VU) for your machine. X and Y value should match.

What post processor are you using? You should use one that has "arcs_inch" in its name. If you use one that just has "inch", your arcs/circles will be segmented moves and can cause poor cuts.

You shouldn't get much if any bit deflection with a 0.5" bit, but if you move too fast, you could get some machine flex. Again, check for machine slop with the motors locked in.

How tight is your PC router? Runout?

Hog the hole and then follow up with a lighter/slower pass to clean it up.

Scott

While you're checking your Unit Values, be sure to check your multiplier values too. Go to: Values > Unit Values > Resolution Multiples for alphaStep Drives, and make sure that they are set to the correct values for your machine. Both X and Y should be the same value.

[donchandler]

I move to the center of the circle and then use the CP command to cut the circle with a spiral down and bottom pass. I use a 1/4" O flute bit. Works well.

[kevbo]

Well after trying for 2 days to figure out the problem, it wound up being a loose set screw on the Y axis motor. This would explain the inconsistencies in the circles and why they appeared oval and irregular. Depending upon how much resistance the machine received (depth of cut, speed, etc), the amount of distortion would change.

Fixing this has obviously improved things greatly but the issues I'm seeing now:

I do a roughing pass which is 1/8" offset to the inside of the circle (the 1" holes I'm trying to make) then on a final cleanup pass, I select Lead Ins/Lead out to avoid a 'plunge mark' at the edge of the circle. The lead in (radius) works fine, but the toolpath does not create a lead out, and as such, at the precise stopping point / where the bit pulls out of the circle, it is visually obvious where the bit comes out - a small round 'nick' is seen at the edge of the circle. I can't figure out how to do a 'lead out'. Is this suppose to happen automatically - ie. lead in and lead out are done with one checkbox?

In regard to the spiraling cut option - is it pretty much the case that PartsWizard 2.0 will not be able to set this up when importing vector data? I know I can CC or CG a spiral cut but this option does not seem to be a possibility when importing vector data? I'm thinking that to get the best circle cutout out of 3/4" MDF, a spiral cut would be the best result with a complete circular cut at the bottom of the spiral.

[beacon14]

If all your circles are the same size you can create a short file that routs the circle you need using a CP command with a spiral plunge and bottom cleanup pass, just as you say. You can even write it so the bit moves back to the center of the hole before retracting.

Then create a drilling toolpath that goes to the center of each hole and drills straight down. Using the SB editor or another text editor, replace all the drilling moves with

FP,(yourfilename).sbp,,,,,2

The bit will move to the center of each circle and the hole will be cut using your custom file with a 2D offset.

You say PartWizard. If you mean PartWorks I can show you how to create a postprocessor that will output the exact code you need with no modifications to the .sbp file needed. If you are using PartWizard, well, all I can suggest is that you look into PartWorks and the other Vectric products.

[kevbo]

Yea unfortunately I did say PartWizard. We've been a 'one trick pony' until recently, mostly cutting larger parts, etc. Partwizard has done everything we needed. I think it will cost me $700 bucks to upgrade to partworks. With the little work right now, I can't swing that at all.

I see the newer bots come with it. From what I'm seeing, peck drilling and spiral cutting are the only 2 features I'd use at this time and for that, it's cost prohibitive.

I will look into what you are saying. From the sound of it, I'll have to figure out all the variables in the comma list of the CC command, import my vectors, then do use a good text editor and do a find/replace type of thing. I've over 500 circles so manually coding would be painful.

For now, what I've done - with the machine back to 'dialed in', I went back to my original Solid Carbide 1/2" upcut spiral, and created 3 toolpaths. 1-drilling centers w/ skin at bottom, 2-offset circle by 1/8" w/ skin at bottom (full .75" depth), 3-finishing cut at actual circle diameter, full depth, with small radius lead in. Results are good for what I need, circles are good, and chip load seems to be nice.

I still need to figure out why there is no 'lead out' when I select the option on a 1" diameter circle.

Thank you all.

[Gary Campbell]

Kevbo...
My machine shipped with PartWizard in 2007. After 6 months I took the upgrade to VCPro (same as PartWorks) and it was worth it. It is even worth it more now. There has just been an upgrade and the features are too numerous to list.

I am sure that you would wish that the 2 features you mention are the only differences, but I am sorry, thats just not true. If you cant justify the upgrade price, thats OK, but I didnt want other users to think that your statements were an accurate representation of the software's features.

For example the spiral toolpath with leads in AND out are in PWks. That would solve your problem. There are dozens more features that are far more advanced than PartWizard has.

[kevbo]

I was not trying to say that that was the only difference at all for the money. What I meant to convey was that for 99.5% of my work, PartsWizard works just fine and to date - the only 2 features I *wish* it had was Peck Drilling and with this latest circles project - the ability to control a spiral downward cut. And to get those 2 basic features, would cost me 700 bucks more.
Partswizard even teases you with the Peck Drilling by showing wording to it in the tool setup - but there is nothing actually there to enter values.

Per your suggestion, I've been looking into the VCarve website and will probably download their demo to take a looksee at it.

Thanks again and sorry for my miscommunication.

[englert]

G-code. Your project seems to be fairly simple in concept. Cut some holes or circles, and cut many, many of them. You may need lead-ins, lead-outs and spirals. All of these concepts can be hand-written in G-Code, which is pretty much a standard language for all CNC's, including ShopBot and Thermwood. Sounds like the circles are the same size, so write the code to cut one circle using the relative coordinate system (G91). Locate the first position referencing your offset position, cut the hole, then offset and repeat the circle in a sub-routine or macro until the first row or column of circles is cut. Then re-locate the head and start the next row or column. This should end up being a rather short program and it can be edited, as needed.

Anyway, you might look into writing this type of program. Essentially, there is no cost other than learning and there seems to be a plethora of help available to you on this forum and at ShopBot.

Good luck and Happy Holidays to All!
Merry Christmas!

Dennis L. Englert
Manager of Product Training
Thermwood Corporation