Why Why Why???

[sevans]

Cutting squares out of Lexan, and the same squares out of PVC. I am using the same bit for both. The only differences are obviously material, and I am not choosing the same tool in the program. However, the tools are both end mills with .25" diameter, same stepover. The only difference is the pass depth and feedrate. Still, the PVC square and the Lexan square are not exactly the same size. They should be. Can someone explain this phenomenon to me? Many thanks. -SE

[Brady Watson]

Is the PVC coming out larger than the acrylic?

-B

[sevans]

No, the pvc is 1/16" smaller than the acrylic. Over, SE

[gc3]

measure bit diameter

[sevans]

it's the same bit

[shilala]

and I am not choosing the same tool in the program.
I'm wondering if this is a typo? If not, I wonder why you'd have two separate entries for the same bit, or type of bit?
Assuming that's a typo, I'd slow the feed rates way down, assuming one material is "springing" under the pressure of the bit, then returning to it's original shape a little bit larger.

To test out that guess, I'd run two passes on the material that's ending up with the wrong dimensions (I'd mic them) and see if the bit takes off any more material on the second go. If not, I'd change the feed rate and try again.
If that doesn't show me anything, I'd guess the smaller piece is tearing out extra material via heat buildup, piling material in front of the bit and taking off more than it should.

Before all that messing around, I'd get out a good set of calipers and see exactly what the heck is going on. Maybe neither piece is cutting to the dimensions you set!

Please let us know what you figure out.

[bleeth]

One toolpath cutting climb and the other conventional?

[dana_swift]

If a different bit is being selcted, it may show "1/4" in the name, but have different numbers in the bit diameter, that will make the parts different sizes every time.

Dave R, has identified the biggest suspect- climb vs conventional. That makes the bit deflections and different material properties most evident.

Cut both parts with the same cut file, and the same bit, see what happens with two different materials. The ideal feed rates for each of them will be close enough to work just fine.

Also polycarbonate (lexan) is VERY flexible (1/4" and thinner) so either a straight edge bit, or down spiral only. Up spirals will lift the material every time. PVC is considerably more rigid.

D

[jerry_stanek]

I'm wondering if this is a typo? If not, I wonder why you'd have two separate entries for the same bit, or type of bit?
Assuming that's a typo, I'd slow the feed rates way down, assuming one material is "springing" under the pressure of the bit, then returning to it's original shape a little bit larger.

To test out that guess, I'd run two passes on the material that's ending up with the wrong dimensions (I'd mic them) and see if the bit takes off any more material on the second go. If not, I'd change the feed rate and try again.
If that doesn't show me anything, I'd guess the smaller piece is tearing out extra material via heat buildup, piling material in front of the bit and taking off more than it should.

Before all that messing around, I'd get out a good set of calipers and see exactly what the heck is going on. Maybe neither piece is cutting to the dimensions you set!

Please let us know what you figure out.

I have 4 copies of the same bit with different speed and cut depth. I just name them for the material I use them for.

[shilala]

I have 4 copies of the same bit with different speed and cut depth. I just name them for the material I use them for.
That makes perfectly good sense, Jerry.
I just edit my tool inside my workpath. I do that because when I started out I found myself changing default bit settings that I knew nothing about, and thought this way I could protect my originals.
I could stop doing that now, but it's become habit. :)

[donek]

The most obvious place to start is to cut the parts with the exact same program. If that produces the same parts, then you need to recreate your original tool paths with a bit more care. If it produces parts of different dimensions, then you have a real issue to figure out.

[sevans]

I have 4 copies of the same bit with different speed and cut depth. I just name them for the material I use them for.

This is exactly what I do as well. That wasn't a typo. I like to track optimal feeds/speeds this way and just select for whatever material I'm cutting.

[sevans]

The most obvious place to start is to cut the parts with the exact same program. If that produces the same parts, then you need to recreate your original tool paths with a bit more care. If it produces parts of different dimensions, then you have a real issue to figure out.

Not sure what you mean. I have already stated that I am cutting the same exact file/same exact bit, and getting 1/16" difference in the overall dimensions. It has already been determined that there is a problem here.

[Brady Watson]

You have two very different material densities, and it is completely possible for the PVC to be larger than the acrylic if you are cutting in a Climb direction - or even cutting one climb and one conventional. If both toolpaths are absolutely the same, this is still possible because the tool can be drawn into the acrylic on a Climb direction cut (since it is more dense) and not on the PVC (assuming Sintra et al) since it is softer and the bit can't bite in as much on climb. Also, if you are using a different physical bit...anything is possible. Assume nothing & take nothing for granted.

-B

[donek]

Not sure what you mean. I have already stated that I am cutting the same exact file/same exact bit, and getting 1/16" difference in the overall dimensions. It has already been determined that there is a problem here.

It sounded to me as it you had generated two different programs using two different tool bits within partworks. If this is not the case, then I am mistaken. I would still open the sbp file in your editor and check to see if they are the same tool path. If the coordinates are different, then you have found your problem. If they are the same, then read on. You could also use the preview screen without resetting and then zoom in tight.

The best way to generate high tolerance parts when machining any material is to produce a roughing tool path that is slightly larger than your finish part and then create a finish tool path to bring your part to dimension. Direction of cut is critical in these operations as well. If you are getting different results from the same tool path, then as Brady says it has to do with bit deflection or the machines rigidity and your cut speeds. I would make your roughing pass a climb cut. Your finish pass should be a conventional cut in plastic. See if that works.

[shilala]

You have two very different material densities, and it is completely possible for the PVC to be larger than the acrylic if you are cutting in a Climb direction - or even cutting one climb and one conventional. If both toolpaths are absolutely the same, this is still possible because the tool can be drawn into the acrylic on a Climb direction cut (since it is more dense) and not on the PVC (assuming Sintra et al) since it is softer and the bit can't bite in as much on climb. Also, if you are using a different physical bit...anything is possible. Assume nothing & take nothing for granted.

-B
That's what I said. ;)

@ Sarah-
Troubleshooting starts at the beginning, and in this case you can easily set up control groups and run the SAME tool file and change the feed and speed settings inside the toolpath.
That way you can rule out the tool file being corrupted, or one cutting in climb and one conventional, or any other number of variables. You want all things to be as close to the same as possible when you figure these things out, trying to use sound and simple principles.
Once you run one of each parts, you can measure them carefully with calipers to see which is actually smaller or larger. Maybe both are wrong?
At that point you'll know exactly what the problem really is; whether it's one of the tool files, or how your feed and speed is reacting on the material.

For instance, if you find that one of the parts is the right size and one is larger than it's intended dimensions, you could run the toolpath on that part again, but at a different feed and speed. Maybe lower than 2.0 ips and around 10,000 rpm. (Less feed speed will exert less pressure on the material.) If you see that more material comes off the part, you'll know it's an issue with your feed, speed, bit selection, or any combination of those things, and that the material is sponging (squishing then springing back) under the bit pressure. I wrote out this scenario explicitly because I think that's exactly what's happening, as I mentioned before, and Brady just explained.

Just be patient, take your time, and gather information that'll make you understand what's happening. Pay close attention to the properties of your material and how it reacts while it cuts. When it's all over you'll be glad this happened because you'll understand your materials more deeply, and that'll help you out time and time again along the way.
Good luck, young lady!!!

[sevans]

You have all been so helpful and I really appreciate it!