Problems with part sizes

[44henry]

I was trying to cut a mortise the other day with the Shopbot and I was shooting for a length of 1.25 and a width of .625 and the numbers I got after the test cut were 1.225 and .600. This isn't the first time I have had trouble getting exact sizes on parts and often I end up just compensating for the difference in the program, but it does puzzle me. I've checked the bits and do not see any size problems, I suppose runout could be a factor, but is there anything I am missing here? Is there some setting that I have overlooked that could make things work the way I think they should? I would like to do some inlay work in the future; however, the problems I'm having with this issue make that pretty much a pipe dream right now. If it makes a difference I have been drawing parts in AutoCAD and than bringing them into PartWizard in a DXF format. Any help would be greatly appreciated.

Alex Johnson

[knight_toolworks]

I battled this for awhile. it is slop in the machine. it changes with direction of cut bit size and cut speed and depth. also material makes a difference. so you need to dial things in a but depending on what your doing.
the only solution is to buy a 50k machine (G)

[shoeshine]

maybe because my machine is new? but I have been making some very small mechanical parts (gears and the like) with tolerences down to 005" - 008" and been having pretty good luck.

2009 PRS BT48 ST

I did have to get a dial indicator on my machine and tweak till I got it perfectly square and plumb.

The Z axis being a perfect 90deg to the table the most important. a fraction of a degree off plumb and the almost imperceptible wobble of the bit threw off my part sizes. I actually drilled and tapped a couple of holes for set screws in my router mount so as to be able to get it aligned.

anyway just my $.02
Chris

[knight_toolworks]

it depends on bit size and cut speed and depth of cut and material. the smaller the bit the less problem the smaller the passes the less of a problem. a cleanup pass really helps in accuracy.

[shoeshine]

Yup I will echo that.

When tolerances are critical, I hog out with a toolpath that is .1 to .05 shy of my final dimension, usually climb at a good rate. Then a final pass cut conventional. I also use the minimum pass depth that results in reasonable cutting times for the parts I am cutting. both strategies to minimize bit deflection.

[44henry]

Thanks, I'll definitely give that all a try.

[ironsides]

Backlash in the Z, Y and Z drives are a big factor also. I used a dial indicator to check my X axis and discovered .070 backlash.

This is easy to fix, just loosen up the stepper motor flange bolts and shove the pinion gears closer to the gear rack.

Then check the fix by giving a .005 command in the +/- directions until all slop is removed.

George

[beacon14]

How are you checking the bit? A digital caliper usually will show that even new bits can be undersized by a few thousandths. Another way to check is to rout a shallow groove and measure the groove width.

[navigator7]

Bent arbor?

[eaglesplsh]

Alex, you didn't mention what type/age machine you're running.

We have a 2009 PRS Alpha. Like Chris Schaie, we painstakingly dialed in our machine with indicators. It wasn't fun, but our parts are within 0.005". If you have a new machine, I'm sure you can get to the same point and it's worth the effort.