Parts 0.050" to big in X and Y

[Scott216]

I just started using the shopbot (full size) my local maker space. I cut some finger joints on 1/2" plywood with a 1/4" down spiral bit. The fingers were 1/2" wide. Unfortunately, they didn't fit together. So I decided to run a simple test. In VCarve Pro I drew a 3x3" square and cut it out of the plywood with the same bit. When I measured it with calipers, it turned out to be about 0.05" too big in both X and Y. Any suggestions on how to track down this problem?

[Brady Watson]

Any suggestions on how to track down this problem?

Yes.

Bring your own tools (bits, end mills etc) to the maker space. The tool you used is most likely a resharpened one. It is important to ALWAYS know the diameter of the bit that is being used and not take anything for granted, such as diameter.

The easiest way to check the diameter is to just run the tool 1/8" deep in a single line & mic the width with digital calipers. You can do this in keyboard mode by toggling on Output 1, hit start to spin the spindle and use the arrow keys to drive the tool in a straight line.

-B

[Scott216]

Yes.

Bring your own tools (bits, end mills etc) to the maker space. The tool you used is most likely a resharpened one. It is important to ALWAYS know the diameter of the bit that is being used and not take anything for granted, such as diameter.

The easiest way to check the diameter is to just run the tool 1/8" deep in a single line & mic the width with digital calipers. You can do this in keyboard mode by toggling on Output 1, hit start to spin the spindle and use the arrow keys to drive the tool in a straight line.

-B

I should have mentioned that I measured the bit with calibers and it measures 1/4". The bit is a relatively new onsrud down spiral - still very sharp.

[Brady Watson]

Rather than play the guessing game, post your file or list all of the parameters you had set for cutting. E.G. - speed, RPM, cut direction, pass depth, was it cut with allowance, how were the parts held down, etc etc.

-B

[Scott216]

RPM: 16000
Feed: 2 in/sec
DoC: 0.25
1/2" plywood - cut 3 inch square - used Profile toolpath on outside of line
1/4" spiral downcut bit, sharp
No cut width allowance
Climb milling - but this is really just a slot, so it doesn't matter
Plywood was nailed down using plastic nails. 3 inch square was also nailed down

I'm headed over to the makerspace this morning to do a little debugging on this. I'll break out the dial indicator among other things.

Here is the shopbot file. I didn't save the vcarve file.

'----------------------------------------------------------------
'SHOPBOT ROUTER FILE IN INCHES
'GENERATED BY PARTWorks
'Minimum extent in X = 0.000 Minimum extent in Y = 0.000 Minimum extent in Z = 0.000
'Maximum extent in X = 8.000 Maximum extent in Y = 10.000 Maximum extent in Z = 0.510
'Length of material in X = 8.000
'Length of material in Y = 10.000
'Depth of material in Z = 0.510
'Home Position Information = Bottom Left Corner, Table Surface
'Home X = 35.000000 Home Y = 24.000000 Home Z = 3.511000
'Rapid clearance gap or Safe Z = 3.510
'UNITS:Inches
'
IF %(25)=1 THEN GOTO UNIT_ERROR 'check to see software is set to standard
SA 'Set program to absolute coordinate mode
CN, 90
'New Path
'Toolpath Name = Profile 8
'Tool Name = 1/4" Down-cut (57-910)


&PWSafeZ = 3.510
&PWZorigin = Table Surface
&PWMaterial = 0.510
'&ToolName = "1/4" Down-cut (57-910)"
&Tool =3 'Tool number to change to
C9 'Change tool
TR,16000 'Set spindle RPM
C6 'Spindle on
PAUSE 2
'
MS,2.0,0.5
JZ,3.511000
J3,4.211820,3.938285,3.510000
J3,4.211820,3.938285,0.710000
M3,4.211820,3.938285,0.255000
M3,4.211820,0.938285,0.255000
CG, ,4.086820,0.813285,-0.125000,0.000000,T,1
M3,1.086820,0.813285,0.255000
CG, ,0.961820,0.938285,0.000000,0.125000,T,1
M3,0.961820,3.938285,0.255000
CG, ,1.086820,4.063284,0.125000,0.000000,T,1
M3,4.086820,4.063284,0.255000
CG, ,4.211820,3.938285,0.000000,-0.125000,T,1
M3,4.211820,3.938285,0.000000
M3,4.211820,0.938285,0.000000
CG, ,4.086820,0.813285,-0.125000,0.000000,T,1
M3,1.086820,0.813285,0.000000
CG, ,0.961820,0.938285,0.000000,0.125000,T,1
M3,0.961820,3.938285,0.000000
CG, ,1.086820,4.063284,0.125000,0.000000,T,1
M3,4.086820,4.063284,0.000000
CG, ,4.211820,3.938285,0.000000,-0.125000,T,1
J3,4.211820,3.938285,3.510000
JZ,3.511000
J3,35.000000,24.000000,3.511000
'
'Turning router OFF
C7
END
'
'
UNIT_ERROR:
CN, 91 'Run file explaining unit error
END

[jerry_stanek]

Are you cutting conventional or climb It could be bit deflection

[Scott216]

Are you cutting conventional or climb It could be bit deflection

It's really a slot, so I don't think it matters. I did have climb selected in vcarve

[Scott216]

I have a 1-2-3 block I'd like to measure on the shopbot using a touch plate routine. Where can I get the script to do this for x and y axis?

[Gary Campbell]

Scott...
The three most common items that cause over/under sized parts are bit diameter, backlash and bit/machine deflection.

Have you measured the bits cut slot in the manner Brady suggested? Make sure you use the same pass depth and feed that you use in the cut file.

"Climb milling - but this is really just a slot, so it doesn't matter" I disagree. Climb mill will push the bit away from a vector, conventional will pull the bit towards it. You can test by cutting the other direction on the same geometry, seldom are the resulting parts the exact same size.

The cut direction exaggerates any backlash (pinion gear to rack looseness), which is the most likely cause of your problem. Your speeds are appropriate, and a solid carbide bit would break before it bent .025" in an inch or so.

Spend your time checking the axes backlash, maybe even with a dial indicator, rather than the 1-2-3 blocks

[Scott216]

I changed the cut depth to 0.1" and slowed the feedrate to 1.0 in/sec. I know I can easily go deeper and faster, but for testing I though I'd baby the setup a bit.

I ran another test with the same bit and the test piece was about 0.025" oversized, a lot better then 0.050" Next I changed out the bit and used my own brand new out of the box Onsrud 57-280. This helped some more, only about 0.015" oversized. Next I switched from climb to conventional and I was surprised at the difference this made. Now the test piece was undersized about 0.005 in X and 0.011 in Y. Gary, you are right about that.

I did measure the slot and it's 0.250"

I put a test indicator on a drill blank I chucked up in the spindle and I was amazed there was almost no runout, well below 0.0001" The needle hardly moved. I had to double check and make sure the test indicator was touching the drill blank.

I haven't tried to look at the backlash yet. I agree, I think a dial indicator would be better then 123 blocks.

So I'm starting to get a feel for this shopbot machine and I'm getting a lot closer to making accurate cuts.

[donek]

When trying to make dimensional parts that must be dead on, you should always make a cleanup cut. This means you first cut the part oversized and then cut it to dimension. This will produce a better part finish and generate less tool/machine deflection. Since you are using a public machine, this will likely be your best practice moving forward. You have no idea how much abuse this machine is seeing, so always assume the worst.

[Scott216]

When trying to make dimensional parts that must be dead on, you should always make a cleanup cut. This means you first cut the part oversized and then cut it to dimension. This will produce a better part finish and generate less tool/machine deflection. Since you are using a public machine, this will likely be your best practice moving forward. You have no idea how much abuse this machine is seeing, so always assume the worst.

That's a good idea. For 1/2" plywood how much stock do you think I should leave for the finish pass, 0.010"?

[donek]

That's a good idea. For 1/2" plywood how much stock do you think I should leave for the finish pass, 0.010"?

It's going to depend on your first cut direction. If you climb cut on your first pass, bit and machine deflection will be away from your finsished vector. You could simply climb your first cut and conventional cut you finish pass. If you conventional cut both passes, you would need to know you machine a bit better, but I would typically use a 0.05in offset on my first pass.

[gc3]

my pass strategy in 1" solid panels...