Thread mill toolpath with regular endmill to add spring passes following helical boring of toleranced hole

[t.g.mandel]

I have a reasonably rigid CNC router and a 2.2Kw ISO20 ATC spindle.

I have been teaching myself the design side of F360 for a while now, and with my machine build finished, am beginning to learn the CAM.

One project I have is to make accurate holes to allow the slip fit of steel locating pins for a vacuum pallet system I am designing. I am having success with the helical bore toolpaths with finishing and spring passes. These are needed to counter the effects of some tool deflection I am experiencing. I recently found some mention of leveraging the flexibility of the thread toolpath, since it allows for multiple finish passes, with varied start points, and both climb and conventional cut options. I have researched how this toolpath works with actual thread mills - such as the pitch diameter offset - but wanted a better idea of if/how it can be used with a regular endmill.

For example, right now I am making a 9.525 mm diameter hole with a 6.35 mm single flute endmill using a boring toolpath and the finish/spring path options it allows. If I follow with a thread toolpath using the same end mill, and choose the hole geometry, is that the same as the thread major diameter? In this novel use case, does the pitch diameter offset have no impact (leave it 0), or would changing it actually lead to more material being removed from the hole? My feeling is that it would not.

Also, I am also experimenting with 2D circular toolpaths, but I am not sure they have any advantage with respect to minimizing tool deflection. I would appreciate any insights and suggestions that anyone cares to offer.

So far I am getting close to having a very acceptable slip fit for the pins, but I am hoping to end up with a 'recipe' that will give repeatable slip fit tolerances while managing the effects of tool deflection on the holes.

Thank you,

Tom

[rengfx]

You need to adjust feed rate for interpolating an internal circle, and it becomes much more critical as you cut holes near the diameter of your cutter. Straight line feed used in a tight circle will not get the dimensional accuracy you seek

Are you controlling for circular feed?

https://www.harveyperformance.com/in-the-loupe/machining-circular-tool-paths/

https://www.youtube.com/watch?v=6wLU97gVo5k

[t.g.mandel]

Thank you very much for the reply and additional insight. I had earlier watched and bookmarked a video - https://www.youtube.com/watch?v=ou5j1R4nNf4 - which at the 3:20 minute mark I believe explains the issue you are presenting. For my testing, I have an aluminum block set up with about 20 holes each of 6 mm and 9.525 mm (these are my locating pin sizes) diameters, and I use each hole to test variations of different tool paths and parameters.

I will check my notes but I believe I did experiment with the adjusted feed rates you highlight. Perhaps I will focus my tests on changing this parameter first, then seeing the results and any further need to use follow up toolpaths to deal with deflection. I just want to eliminate (reduce?) any 'conical' holes. With my 24K RPM high speed spindle, I only feel comfortable going down to about 10K RPM, so I try to be mindful of that while watching SFM and chip loads. The various formulas and parameters are stating to make more sense, but they are not yet intuitive - I am hoping that will come with more hands-on milling experience.

I would still like to explore toolpath options that allow me to mill from the bottom up, with options of more that one finish and spring pass. For now one strategy that also helps is repeating the bore toolpath a second time.

Thank you again for helping.

[t.g.mandel]

After more experimentation I believe I have a recipe that will work given the limitations of my set-up. 

I am not pursuing the thread mill option, as I have found no information on exactly how changing the various parameters will impact the cut. That, and it really is not the correct solution, although perhaps a novel approach.

My final strategy is giving me good results, with slip/clearance fit tolerances that are better than expected with my hobby CNC. First I use a 2D boring operation with an O flute endmill, and a finish and repeat(spring) climb pass.

The second operation is a 2D circular operation. I used a small - 0.5mm bottom height offset, and two repeat conventional passes with a negative radial stock to leave. I also left multiple depths unchecked so the two passes are at full depth/radial cut (minus the bottom offset value), which is why I was originally exploring the thread mill toolpath.

My 3/8" steel pins seem to be slightly undersized - purchased off Amazon - but most information on fit/tolerance standards say that pins are usually slightly oversized. I found that my negative radial stock to leave trials of -0.04 mm to -0.08mm are close (if not a bit higher) to those in the tables I found. It is possible therefore that I am not milling holes that are truly 3/8" (9.525 mm), but I do not have the tools to accurately measure their inner diameter. Regardless I believe this will definitely work for me and the vacuum pallet I am designing. Not only the slip fit for the pins, but I am also confident I can mill the friction fit holes I need for the steel bushings.