Dimensional accuracy when cutting plywood

[rcbrust]

Just got my Desktop last week and started out by cutting some modeling parts out of 1/4" aircraft grade plywood (Midwest brand). The issue I'm having is if I, for example, cut a 3.000" diameter circle it measures about 10 thousandths over once cut. I tried adding an extra final pass and this hasn't seemed to have any effect. Is there a "springiness" issue with wood or am I expecting too much from the machine?

I've tried it with multiple bits, both 1/8" and 1/4", and there is no difference. I'm thinking of setting the bit diameter 20 thousandths smaller but before I do that I thought I'd ask here to see if you guys have any ideas.

Thanks,
Randy

[Gary Campbell]

Randy...
Are you cutting in "climb mill" direction? Try cutting "conventional". This may result in part dimensions that are too small. Half the difference of the size variation is your deflection and/or bit diameter inaccuracy.


OR, you can simply set the bit 10 thousandths smaller. That should get you a lot closer. Of course wood can expand and/or contract when cut, and bits seldom cut the exact diameter they are sold as. (Do the math)

[rcbrust]

I'm cutting in climb. I was thinking of reversing the direction of the extra last pass to cut in conventional to see if that helps. I'll report the result.

Randy

[scottp55]

IF the bit measures exactly the same as entered in the tool database, and results are the same with different bits...
then perhaps simply use the allowance offset till it's as close to perfect as wood gets?
DOUBT it's Desktop's accuracy:) :)
scott

[pro70z28]

I've run into the same problem cutting metal parts. I solved it by cutting slow, making sure the bit was the actual size it was advertised as and if that wasn't working i'd dial it in by giving the bit an adjusted diameter.

[JimDav]

I'm cutting in climb. I was thinking of reversing the direction of the extra last pass to cut in conventional to see if that helps. I'll report the result.

Randy
It will make a difference. Climb cut tends to pull fibers out. Conventional tends to push them in. First thing the guy I bought my Bot from taught me was to use climb first, leaving an onion skin. Then come back and finish with a one pass conventional cut all the way through. For several reasons, it also give a smoother final cut.

[rcbrust]

Yeah, I'm definitely going to try leaving about 5 thousandths and then run a final pass the other way.

Dimensional accuracy of the bits has been brought up. I was assuming that the bit diameters were fairly accurate, like within 1 thousandth or so. Are there any brands that are known for their accuracy over other brands?

Randy

[Gary Campbell]

In many cases it is not the bit "actual" diameter that matters. It is the size of the cut that bit imparts on the material. In every case, when sub .010" accuracy is required, I would suggest making a 1"/sec cut 1/8" deep in the material you will use and using a digital caliper measure the actual slot that the tool cuts. That way you will know what diameter your material thinks the bit is.

You also don't mention what feeds/speeds/pass depth you are using. On a small machine like the desktop aggressive cutting will deflect the cutter, towards the vector when using conventional direction and away from the vector when using climb. This shows up the most on hard materials

[dlcw]

When cutting plywood, that I needed really tight accuracy on, I first cut in a climb direction leaving a 1/32" skin. This will push the bit away from your cut line. I then do a conventional cut in one pass thru the skin. This will pull the bit to the line. I've had really good luck using this method. The beauty is in the software you can save both toolpaths in the same file, if the bit being used is identical for both cuts. When doing a large sheet of parts, I do the first pass leaving the skin on all the parts before doing the final conventional pass.

Another thing to consider is that wood, even plywood, will relieve internal stresses, when cut, that can cause the plywood to move dimensionally. I know of no way to eliminate this issue for .001" accuracy in a wood part, which the machines are capable of. Wood, even plywood, is a moving medium to work with. Just the nature of wood.

[Gary Campbell]

I had a number of emails regarding my last post. So to clarify, I did not mean that the bit was deflecting. For all practical purposes, they don't. I meant that the machine was deflecting which forces the cutter into or away from the vector. "Failure of the machine to withstand the forces generated by the bit, allowing it to vary from the cut vector".

[Brady Watson]

On a small machine like the desktop, aggressive cutting will deflect ̶t̶h̶e̶ ̶c̶u̶t̶t̶e̶r̶ the machine, towards the vector when using conventional direction and away from the vector when using climb.

There I fixed it for you.

(Gary already knows everything I mention here...it's posted for others)

Quite often the cutter is to blame for 'deflecting' when parts come out too big/small - and in reaility, carbide doesn't deflect, or bend. Being crystalline and stiff, it will just snap clean off...unlike HSS, which is great for aluminum and other dense materials where you want it to deflect a little (to resist breaking and absorb harmonics). Deflection DOES happen but it happens because of what it's attached to, the structure of the machine...not the cutter on its own. Wait...what? Read on...

It's also probable that microstepping, with its inherent hyteresis (aka willy-nilly slop) between 1/4, 1/2 and full step torque detents that there's some 'electronic backlash' to contend with here as well. Did you know that when a 1/10 microsteppping drive is hooked up to a stepper that it will deliver only 15% of the advertised nameplate torque when at a microstep position? Stop and think about that a moment...especially as it relates to parts cutting off-spec. (then subtract 50% of the 15% for drives that do current reduction when the motor is stopped and supposed to be holding postion...what's that 7.5% of nameplate torque?)

The DT, for reasons I can only imagine, doesn't have the most well thought out mechanical reduction at only 2:1 on the screw, which doesn't help with cutting torque. The single screw in the Y doesn't help either...which can cause each end of the gantry to do the watusi. You have to make provisions for these things - meaning, make sure your RPM is high enough, your MS is slow enough (somewhere between 1-2 inches per second) to keep the chipload light enough not to deflect and not to lose steps. Once you learn where the reliable speeds/feeds are, you just learn to run in that range - and can get some nice accurate cuts on these machines. If I were designing the DT, it would have 5:1 ballscrews, higher torque motors and a motor on each side of the gantry...but that's me.

I know few reading this spent the paltry price of entry for a dial indicator with magnetic mount ($30-ish) - It is one of the most useful tools in the shop once you understand how to use it. For those that do have one, put it on the machine and preload it to the table/bed. Then ever so gently press down on the gantry in the middle. It is scary how much these lightweight tools deflect under the smallest of pressure. See for yourself...PRS, PRT doesn't matter. Some are better than others...only through instrumentation (like an indicator) can you track down the source of slop or over/under sized parts after you've eliminated the obvious.

Others have made good suggestions about getting accurate cuts - check climb vs conventional, rough cut it with allowance then shave it to final size etc. All very good pointers....but the reason you have to do that in the first place is because the machine either needs maintenance (v-rollers adjusted, rack to pinion lash etc) or you've just reached the limits of the machine chassis/structure itself. In the case of the later, slow things down and lighten the chipload. Adjusting VR to soften abrupt moves also helps.


I've run into the same problem cutting metal parts. I solved it by cutting slow...

Case in point...machine deflection. Don't take my word for it though...buy an indicator and see for yourself. ...unless you're one to believe that ignorance is bliss ;)

-B

[rcbrust]

I tried some more test cuts last night. When I first posted, I was cutting 3.000" diameter circles and they were measuring between 3.010" to 3.012" depending where on the circumference I measured the diameter. This time I did the usual multi-pass climb cut but with a 10 thousandths offset and then went back and did a final full depth conventional cut to the final dimension. Measuring the diameter at various locations, I was getting 3.000" +/-0.002". Much better than before. I may try adding a second final conventional pass just to see if that makes any difference.

Thanks for all the tips guys.

Randy

[bill.young]

Just to clear up one thing, the Desktop MAX has always had drives on each end of the gantry, and the Desktop added the second motor and drive not too long after the MAX came out.



I tried some more test cuts last night. When I first posted, I was cutting 3.000" diameter circles and they were measuring between 3.010" to 3.012" depending where on the circumference I measured the diameter. This time I did the usual multi-pass climb cut but with a 10 thousandths offset and then went back and did a final full depth conventional cut to the final dimension. Measuring the diameter at various locations, I was getting 3.000" +/-0.002". Much better than before. I may try adding a second final conventional pass just to see if that makes any difference.

Thanks for all the tips guys.

Randy