[maker4444]

My interpolated holes are slightly smaller at the bottom.

So a cylinder that will slide in snuglly from the top won't fit from the other end of the hole.

I don't think this has anything to do with deflection because tried multiple finishing passes.

If the spindle were running out, that would make a bigger hole.

If the spindle were at an angle, the hole wouldn't taper.

So what's going on? Does this mean that the milling bit is smaller at the tip?

[chuckorlando]

You left out a lot of info.

Material, depth, speed/feed, tool flute length and size, etc.

Look at the code. If it is boring the same size hole with the same locations that should be reflected in the code.

I would bet it is tool push off. Or the finishing strategy you are using. I like to do a helical bore with more flute length then needed. Or a reduced shank tool. If the flutes go lower then the bore the shank will push off the tool. I suspect the problem here

[maker4444]

You left out a lot of info.

Material, depth, speed/feed, tool flute length and size, etc.

Look at the code. If it is boring the same size hole with the same locations that should be reflected in the code.

I would bet it is tool push off. Or the finishing strategy you are using. I like to do a helical bore with more flute length then needed. Or a reduced shank tool. If the flutes go lower then the bore the shank will push off the tool. I suspect the problem here

Hmmm. I think you may be right.

6mm endmill, the 23mm diameter and 20mm deep hole was hewn out first with a twist drill, then a helical strategy, then with circular passes (then repeated). All at very conservative speeds.

Attached is a photo of the tool. Is the flute length to be read as being 11mm or 21mm (as measured with my calipers)?

ps tried with code from two different sources (fusion360 and USBCNC).

[chuckorlando]

11mm is the cutting length of the flutes. So over 11mm the shank is pushing off the wall. Rubbing.

[maker4444]

Brilliant.

Thanks a lot @chuckorlando !

btw. for getting the most accurate interpolated holes with an endmill would you recommend a longer flute length - or a narrower shank?

[chuckorlando]

Longer flutes leaves more material for rigidity.

[maker4444]

Thx.

[chunkymonkey]

Also consider, when helical ramping thru hole, that the bottom of your tool will wear faster than the top. After a bit, you will see taper from this also. I'd throw in an extra tool just for finishing to give you even more chances for success.

[maker4444]

Good thinking @chunkymonkey.

I can use up some of my too-short endmills ramping holes.

Could have carried on making the same mistake for a long time if this particular part hadn't come up....

[chuckorlando]

If you can, you could drill the hole. Then finish in one shot with end mill at depth.

[maker4444]

Hmm things have improved but the problem hasn't gone away. This is turning into a mission.

Have tried on 3 different machines, with different bits and different sources of Gcode.

At best the 20mm hole is 23.08mm at top when 23.00 mm at bottom.

Could it be that the bit tends to shim off the top of the hole slightly, even when the contact is from a fluted region and not the shaft?

And yes I do an extra finishing pass such that I can hear no further material is being removed. And have tried both full depth passes and stepping down circular passes at 1mm intervals.

And now only lightly tighten the vice (the part is held low down).

Do other people notice similar effects?

Am using mist coolant / compressed air.

[chuckorlando]

Before you do the spring pass, what is the doc and woc you are taking?

[maker4444]

In the beginning I was:

- drilling with 12mm twist;
- then switch to a with a 6mm or 12mm flat bottomed 2 flute endmill;
- helical boring to leave 0.1-0.2mm;
- doing a circular pass with 1mm stepdowns to remove the rest;

Now tend to:

- do everything with a 2 flute 8mm endmill;
- 3d adaptive clear with 6mm stepdowns and a helical ramp with each stepdown; leaving 0.1mm at the end;
- remove the rest with two stepdowns;

[chuckorlando]

Are you using an adaptive to finish or just rough it?

Seems like just deflection or tool wear.

[maker4444]

Thanks @chuckorlando.

In all cases:

- finishing has been clean circular passes;
- bits are new and have tried different ones;
- the adaptive clearing (Fusion360, 3D adaptive) is a roughing strategy; that being said I've done it as slowly as possible as per Gwizard "fine" setting;

If it were deflection then doing a second circular finishing pass should fix it. Instead it takes nothing off.

If it were tool wear it shouldn't happen with new tools.

[chuckorlando]

In theory yes. But your hole is already over sized if I remember the numbers correct. Maybe it's pulling the tool into the work? Causing a bit over sized hole so the spring cut is air

Can you post the code? Or at least look at it and see if the code has a issue. I doubt it's the code though

[chuckorlando]

I use HSMWorks. It's F360 in solidworks. I was wondering if you finished using adaptive because the arcs produced. Not the best for finishing.

[maker4444]

The numbers I gave were 23.08 at the top and 23.00 at the bottom. Achieved that because progressively increased the diameter in CAD to try to get the bottom up to 23... which left the top then too big.

Attached is a typical Gcode for doing the finishing with two circular passes on a precisely 23mm hole.


So far I can only imagine two ways that the hole could physically taper towards the bottom:

1) the idea below that the shank was shimming off the top of the hole => sounded really good but, having changed bits and strategy doesn't seem to be that;

2) if the bit/collet was both off centre and pointing towards the centre then it might spin to create a cone-shape => but I measured the runout of the bit just below the collet and it's very small, just a fraction of the 0.01mm (maybe 0.003mm?) intervals on my dial test indicator;

Confused.

[chuckorlando]

If the J's match on the g17 plane you should be ok.

I wont lie, MM are not the norm for me so excuse any numbers I might say that are just stupid ahaha.

I believe we should maybe try a new approach. Can you rough the whole and leave .01 or .02in on the wall. (What ever the tapper is plus a cunt hair), then do a finish opp at full depth One pass.

[chuckorlando]

Run out would not cause a tapper. It would cause an egg. Even a head out of tram would not tapper a hole. Well it would but on one side it would tapper in and the other it would tapper out.