Bit and program accuracy

[richard_saylor]

This is a two part problem.
First off, I'm having troubles finding upcut spiral bits that are actually .5 inch. Most range from .49 to .495 inch. This includes Bosch, CMT, Whiteside, MCLS and various other brands. Yes, my caliper seems to be accurate because it measures the shaft size on all my .5 inch bits to be exactly .5 inch. The bits are bought from reputable dealers and are not marked as seconds.
Secondly, what kind of accuracy should I expect when cutting a pocket toolpath. Knowing that a bit is .495 inch, I can either designate a new tool with this cutting diameter, or selecting a virtual .5 inch tool and alter the drawing to obtain the proper size. Using the second scenario, if I want a circular pocket toolpath of 2.2 inches with the .495 inch tool, wouldn't I give the pocket a 2.21 inch diameter? With experimentation, I must give it a 2.226 inch diameter toolpath to obtain the 2.2 inch hole.
To test the accuracy of my inside vs. outside caliper, I've measured the tip of the tool and then cut a .25 inch deep path through hardwood and measured the width of the cut with the inside caliper. The widths are exactly the same.
Any ideas?

[ssflyer]

Unfortunately, I've been finding this to be more prevalent, lately. My Onsrud bits seem to be a bit better, in this regard. So I simply add my tools to my database for the tool, itself, with the correct diameter. Kind of a pain, when you've got several, with differing diameters...

[richard_saylor]

A follow up on part two of my problem.
I created an End Mill tool of .495" to model exactly the diameter of my physical End Mill. I created a 2" circle. Using the .495" tool I created a Pocket Toolpath inside the 2" circle.
After routing the circle, I measured and the pocket is 1.98". Am I expecting greater accuracy than the ShopBot can accomplish, or is it something else?

[MogulTx]

You have to also know how the material is going to react to your bit. If you tell the software that it is a .495 bit, there may be the issue of not measuring the bit to the most extreme diameter of the bit. ( In other words, it may be cutting a larger path than what you are expecting, and so it may, in a cutting-outside-the-line application, leave you with a slightly smaller diameter. If cutting inside the line, it may leave you with a slightly larger diameter.

Sometimes the material will encroach /swell into the cut path due to swelling out of the grain of the material being cut (foams sometimes do this, as do woods- especially those that are still green or have a higher than expected mositure content.) Also: many things will temporarily expand from the heating /trauma of the material from the cutting process...

You may need to investigate a little bit to figure out what issue you are having and to pin it down a little further!

I measure bits all the time that measure out at .116, but that cut like .125. I am trying to figure out how it does it. I figure it is becasue the spiral is slightly off center and I am not measuring the true diameter of the bit, but rather the offset bulk of the cutting faces, which are not necessarily symmetrically laid out on both sides of the centerline of the bit...

[richard_saylor]

As stated in my first post: "To test the accuracy of my inside vs. outside caliper, I've measured the tip of the tool and then cut a .25 inch deep path through hardwood and measured the width of the cut with the inside caliper. The widths are exactly the same." From this, I would assume that my measurement of the bit is right on.
As far as type of wood and any resulting swelling, I get the same results from pine, bone, plastic and Ipe.
My need for accuracy comes from doing inlay with various materials and other interference fit parts for my guitar business. The tendency for the machine to cut pockets too small and profiles too large, compounds the error. I'm constantly having to experiment with my drawings to get things to fit.

[gc3]

spindle runout, bit deflection, machine backlash could also be factors

[richard_saylor]

"spindle runout, bit deflection, machine backlash could also be factors "
Doesn't it seem that all of these would create a larger cut rather than a smaller one?

[bob_reda]

If it is consistent it could be that your unit values may need tweaking. Also, I don't know what software you are using. I use aspire and for inlays I use the same bit for both the male and female.

Bob

[richard_saylor]

Bob,
I'm using Partworks. It's turning out the correct numbers, I've looked at the sbp files.
I can't use the same bit to pocket ebony and then cut out MOP or abalone laminates. A simple test can be done with the same bit, though. Cut a 2" circle and a 2" circular pocket in plastic with the same measured bit. Shouldn't they fit perfectly, maybe with a bit of interference? My circle will always be .004" too big.

[bobmoore]

Richard. It can be frustrating at times when your needs are greater than your experience or machine capabilities allow. There is an allowance button in the profile toolpath area that will accommodate slight differences in tool diameter. If you are really under the gun you can send some of your material to the good tool houses and they will run it on their machines to verify feeds, speeds, diameters, ect. I know vortex in Schofield, WI will do that and though I haven't dealt with him yet Gary Beckwith on our forum probably would too. I would expect to pay a fee for such service. If you want more help from the forum for this it would help to include a lot more information about your setup. Are you climb or conventional cutting, feed and speeds, hold down system, what machine model?
Bob

[donek]

What Bob said.

If you are looking to get to within a few though, you need to make a roughing pass and then a final cleanup pass that takes of between 0.02 and 0.05in. Even then, to expect this sort of accuracy from a router is going to require you spend a great deal of time fine tuning your machine and your process. There is a reason high tolerance parts cost more from a machinist. They take time and patience to make and dial in. When I'm trying to get this close on a part, I produce a 1st article, measure, and adjust the allowance offset until it is where I need it. You're better off designing parts and processes that are robust enough to handle a certain degree of inaccuracy.

[gc3]

'It can be frustrating at times when your needs are greater than your experience or machine capabilities allow"

welcome to the jungle...

so... cut circle .004 smaller or

whatever it takes to make parts fit

[bob_reda]

Bob,
I'm using Partworks. It's turning out the correct numbers, I've looked at the sbp files.
I can't use the same bit to pocket ebony and then cut out MOP or abalone laminates. A simple test can be done with the same bit, though. Cut a 2" circle and a 2" circular pocket in plastic with the same measured bit. Shouldn't they fit perfectly, maybe with a bit of interference? My circle will always be .004" too big.

Richard,

I've done a lot of inlays, especially letters, not out of bone or ebony, but using the same tool, which by the way, Vectric illustrates several times on their tutorials for inlay, I always allow .02 allowance on the female part. All my inlays have always fit. I didn't measure them, nor my bits, so if I needed a precise size I would probably do some tests like you are doing and make the necessary adjustments. The only time I have trouble is when, by accident, I use different tools for one part or the other. Shopbot claims- Positional accuracy of +/- .002” on their alpha equipment. That seems to be about .002 for bit runout, router or spindle runout, backlash and the rest.

Bob

[MogulTx]

Cutting a straight line and cutting a pocket are two different functions. On the first, you are guaranteed to get the size of the bit because the bit can't cut smaller than itself. On a pocket, you are using multiple passes to make the recess you want... I have done inlays with all three of my machines- and have not had a problem. As I recall, I always added a small margin to my pocket to ensure the part would fit. I was inlaying mahogany into maple. I did several tests to get the best and tightest fit. I think Bob's suggestion of a .009 is about as small as one would want. That is very close to needing a press fit in the machining world- and you are working with fairly fragile natural or man-made shell sections. If I were gluing them up, I would want a modest slip-fit, not a press-fit.

[MogulTx]

Sorry. I fat fingered that. Bob did not mention .009. I should have written that I have used as tight of a fit as .009 and had to tap the components into place. I think the .01 or .02 is probably a little more where you might need to be. Since inlays are thin, there should be little trouble with the differential you can get by having them at an angle while inserting.

[chiloquinruss]

"or whatever it takes to make parts fit ", since I don't do steel just wood or plastic I have to allow some room for the glues used to put stuff together. Whatever the bit does or cuts is what I use after I do a test cut first. Doing inlays I just use what ever the Vectric software tells me to do. On one occasion I did use the .02 offset as was mentioned above but that was glue related to the inlay I was trying to do. Russ

[richard_saylor]

Thanks all for the wealth of experience!
I am always nudging and making allowances and often find myself using intuition more often than logic.
Sorry about my 'lack of experience' and high expectations. I guess it comes from being a structural engineer, software programmer and technical CAD professional for the last 25 years.
Ahh, the curse of overeducation.

[richard_saylor]

I'm going through all my bits and creating virtual 'tools' to match their actual widths and angles. I've decided that subtracting .002" from the measured diameters will get me my intended results in most cases. It's also a easier fix than going through hundreds of files and tweaking allowance offsets.
While cataloging my bits, I found an NOS CMT set of five upcut spirals that all measured exactly to their advertised specs. The newer CMT bits are all undersized.

[scottp55]

Had a machinist in yesterday to check out the Desktop, He had never seen a cnc that small and has never worked wood in his life. He asked to see the bits I would be using and showed him the sb starter set and a few others that have been dribbling in, almost every spiral and straight was .002-.003" undersized. the only one that was dead nut was a .5" straight from Leigh that was 10 yrs old. I may do what you've done and create a virtual category.