Please Cut This Pattern

[Bonch]

I have been trying to make a part for a friend of mine and for some reason I cannot get it to come out right. I have calibrated my machine several times and the sizes never come out right. I have measured my bit and even tried ramping and a finishing cut around the outside and the dimensions are still wrong. I put the measurements in the file to make it easier to see what I am doing wrong. I am hoping someone will cut this out and see if maybe I made the part in Aspire incorrectly. The material thickness is adjustable based upon whatever you have as scrap. I hope it is just something stupid but am afraid I have something amiss in my machine.

Thanks for the help.

[metalworkz]

Does this preview look correct for what you are trying to cut?

[Bonch]

Yes that is it. It cuts fine just the dimensions are off when I cut it out so not sure if I designed it incorrectly, set up the cut wrong or my machine is not cutting correctly for some reason.

[highpockets]

I get the same preview as Wes. Using your dimensions some of your circles are off by .001". What are your measurements of the part when you cut it out? What material are you cutting?

[metalworkz]

I am inclined to think it has something to do with your machine. Maybe motor tuning, and then if that is not the problem check the motor couplers and make sure they are not either flexing or if locked with set screws that they have not become lose at the shaft. If locked with set screws it is a good idea to file a flat on the shaft where they lock down so they can not slip or move during direction changes. I have experienced a lose set screw on my Syil mill that was causing circles to cut 'egg shaped'. Also if there is a bind in the slides or the axis it can cause problems with the cut as well as any racking if using a gantry type machine. After using the Vectric software for some time you will realize in most cases these types of problems are machine related and the software is not the problem. I will agree that problems of this type are not nearly as easy to pinpoint as some other problems and I had a problem with my Z axis that confronted me for a long time before I opted to replace the Z axis slide and ball screw with an actuator and that seems to have corrected the problem. Maybe make a list of the possible causes and eliminate them one at a time and check them off so you have the list to refer to as you work towards the solution. Not knowing the exact discrepancies does not help us try to mention solutions so if you can add more detailed information like what dimensions are off and in what direction related to the axis as it is being cut it will help pinpoint things better. Hope something here helped but a lot is like trial and error until you find the culprit/

[Bonch]

I get the same preview as Wes. Using your dimensions some of your circles are off by .001". What are your measurements of the part when you cut it out? What material are you cutting?

This cut was in .725" plywood. However it cuts about the same in pine. Measurements are in the attached pdf.

[highpockets]

I get the same preview as Wes. Using your dimensions some of your circles are off by .001". What are your measurements of the part when you cut it out? What material are you cutting?

This cut was in .725" plywood. However it cuts about the same in pine. Measurements are in the attached pdf.

You're using softwood, softwood never measures well. But you should be getting closer that the measurements you've posted.
What is your cut depth per pass and how are you holding the part down. Also what is your feed rate?

[Bonch]

I get the same preview as Wes. Using your dimensions some of your circles are off by .001". What are your measurements of the part when you cut it out? What material are you cutting?

This cut was in .725" plywood. However it cuts about the same in pine. Measurements are in the attached pdf.

You're using softwood, softwood never measures well. But you should be getting closer that the measurements you've posted.
What is your cut depth per pass and how are you holding the part down. Also what is your feed rate?

.125 DOC, 50 in/min. Using clamps on 4 sides.

[highpockets]

.125 DOC, 50 in/min. Using clamps on 4 sides.

What's the size of your cutter. Assuming an 1/8" or 1/4" end mill, your DOC and feed rate are fine. At this point I'd start really looking at your machine.
If you cut out two pieces are the measurements the same?

[Bonch]

1/4 inch endmill. If you dont mind and have some time could you cut it out on a scrap and make sure it carves correctly. I hate to tear down the machine if it is something stupid I did in the design.

[highpockets]

1/4 inch endmill. If you dont mind and have some time could you cut it out on a scrap and make sure it carves correctly. I hate to tear down the machine if it is something stupid I did in the design.

I would do that in a heartbeat, but I'm on the road until the middle of next week.

[cac67]

1/4 inch endmill. If you dont mind and have some time could you cut it out on a scrap and make sure it carves correctly. I hate to tear down the machine if it is something stupid I did in the design.

What is the actual measured size of the 1/4 endmill. Likely not exactly .250000.

[IslaWW]

Something to remember....
In many cases an endmill will measure an exact size, .250 for example at its shank. It may measure close to that across the flutes, if one is good with a caliper. That said single and 3 flute bits cannot be measured by calipers.

If you need to know what your wood thinks the bit diameter is, cut a low feedrate (~30-60 ips) slot 1/8" deep and measure the slot. You may be surprised at the results. What may also surprise you is that the slots in various materials may also vary. Materials of varying densities will return different results with the same bit. The actual width of the cut should be entered into the design software to ensure the most accurate cuts.

[TReischl]

I am going to toss something in here. . . . after reading your PDF with the "errors".

Measuring small holes is not something that is real easy, especially in wood. It is not even easy in metals, that is why they make plug gages, very accurately ground.

Wood. It has grain. It does not cut the same across the grain as with the grain.

If I am looking for a very precise hole I first rough the hole out. Leaving about .010 all around. If you cut a hole with a .25 end mill with a 50% stepover you are going to get deflection. It seems that many of us seem to think that if the tool is told to go down a path then by gosh it is just going to go right down that line never mind physics, like deflection.

Way, WAY back, like in 1975 I programmed a Pratt Whitney NC lathe, big, hefty, massive machine. Even using 1 X 1 tooling we always took a "finishing cut" to get accurate results.

But, since we are now so lazy, it is way too much effort to program the hole a bit undersize and then generate a final finish cut in a separate tool path. It is really difficult to do, one has to use the Allowance Offset box and type some numbers in, like .010, then calc the path, then OMG, select the geometry a second time and select Profile and click a few more times on the mouse. It is a lot to do!

Seriously, try doing a finish path and see if your results are not better. I am on an earlier version of Aspire so I cannot open your file to see if you used a finish path or not, but no one mentioned it so I thought I might suggest it to you. BTW, if you use the Ramps/Spiral option when setting it up you will get a really nice hole.

Here is the thing, I notice your measurement discrepancies are both plus and minus, this tells me that the measuring technique might be suspect, or that you measured across and with the grain. If you are using a dial calipers to measure holes, well, ok, but do not think that you are going to measuring with an accuracy of +/- .002 or anything even close to that in wood. Those little inside edges are quite narrow, a little pressure and you can make the hole all sorts of sizes.

Here is another tidbit, I am feeling chatty this evening..... Buy a small piece of .50 inch drill rod, it is not very pricey. But it is quite accurate in terms of size and roundness. Use it as a gage. A lot of rods, just run of the mill stuff are also very accurate. Brass, aluminum, steel. You can use pieces of that stuff as gages.

[Leo]

Buy a small piece of .50 inch drill rod, it is not very pricey. But it is quite accurate in terms of size and roundness. Use it as a gage. A lot of rods, just run of the mill stuff are also very accurate. Brass, aluminum, steel. You can use pieces of that stuff as gages.

For that matter, Class "Z" pin gages are generally under $15 each for sizes under 1" diameter. Tolerance on Class "Z" is more than adequate for wood. I agree - best way to measure a hole.