Any suggestions for helix boring hardened A2?

SigurdACVW · Mar 27, 2021

I have a part made of hard A2 with an array of 50 1/4" dowel holes, .250 deep. It's a fixture. The holes have been roughed out to .240". Jig grinding is not an option due to the cost. Wire EDM is not an option due to the holes also having 10-32 threads in the bottom. If I were to helix bore these (understanding that the mill will not hold the size and position that a jig grinder will), I'm thinking of using a .125" 7-flute TiAlN-coated carbide EM, 150 SFM and .0005" chipload. What I'm stuck on is the pitch. What is a reasonable value to use? Do you have any other suggestions that might help here?

cameraman · Mar 27, 2021

SigurdACVW said:
I have a part made of hard A2 with an array of 50 1/4" dowel holes, .250 deep. It's a fixture. The holes have been roughed out to .240". Jig grinding is not an option due to the cost. Wire EDM is not an option due to the holes also having 10-32 threads in the bottom. If I were to helix bore these (understanding that the mill will not hold the size and position that a jig grinder will), I'm thinking of using a .125" 7-flute TiAlN-coated carbide EM, 150 SFM and .0005" chipload. What I'm stuck on is the pitch. What is a reasonable value to use? Do you have any other suggestions that might help here?

Just out of interest what machine are you running this on ?

Or type...

Any sense of the actual hardness of the material / A2 ? Or surface hardness vs. hardness deeper into the material ?

Scruffy887 · Mar 27, 2021

Just a WAG. Emill at 2xD may deflect and taper the hole. I would relieve the un needed cutting edges further up the flutes to prevent deflection by rubbing. Pitch will tell you how much cutting edge you will need.
Your results may vary.

SigurdACVW · Mar 27, 2021

cameraman said:
Just out of interest what machine are you running this on ?

Or type...

Any sense of the actual hardness of the material / A2 ? Or surface hardness vs. hardness deeper into the material ?

It's hard throughout. Machine cutting it will be a Haas MiniMill 2.

Scruffy887 said:
Just a WAG. Emill at 2xD may deflect and taper the hole. I would relieve the un needed cutting edges further up the flutes to prevent deflection by rubbing. Pitch will tell you how much cutting edge you will need.
Your results may vary.

Thanks. I appreciate it.

This part is 6" x 5" and 1" thick. All sides will be finish-ground. It will be used in the shop for holding/milling/grinding and inspecting small or non-ferrous parts.

Like I mentioned earlier, the initial intent was to jig-grind the holes so they were straight with the outsides of the block. The cost eliminated that as an option.

Plan B is milling the holes, and then for something that REALLY needs to be there, indicate two dowels. Which brings me to Plan C. If I can't trust the holes and I'm going to be indicating anyway (the aforementioned Plan B), do I bother with dowel holes at all?

Nagol · Mar 27, 2021

Your size will probably go to crap in a hurry milling it like that. You should just circle mill it. Using more of the cutter at a time will always give you better life of which will be limited in the hardness material you are using. Depending on how critical your hole size is I would recommend just using a rougher and a separate finishing endmill. If you are going for a press fit mill .002 under and finish in one pass. If you are going for a really tight slip fit run each hole twice in one pass and you should have no problem with size. As far as tool I would recommend a Gorilla Yeti in 3MM or 1/8 size running at 250 SFM and .0015 IPR. Using 2 of these I'm sure you will get through the part with no trouble. I recently made a bunch of fixtures in mild steel doing it this way. .6255 hole over a 1/2-13 thread and I ran 800+ holes with no adjustment using a 5/16 tool. Rough and Finish in one pass. Run 2 finish passes if size is super critical.

Milland · Mar 27, 2021

I'm not clear on the design of the fixture (are the parts to be checked supposed to fit over all 50 dowel pins?), but you might look at "fake" jig grinding using your machine, using 3/16 CBN grinding pins for the final ~.001 and to true up the hole after milling it closer to final size.

These guys offer some cheap (but I think not junk) CBN pins, a 1/8" shank, 3/16" head, and 1/4" LOC pin is only $16:

CBN Pins, BL Series | Gesswein

Use whatever method/endmills to semi-finish, then helix in with these pins for the last bit and to true the hole. You'll need to establish parameters, but likely just max the spindle and take ~.0004/pass (diameter) until you hit size.

Sure, you'll have to feed slowly, and if your machine is sloppy the results will be suboptimal, but it should give a more consistent final bore since you can ignore (sorta) carbide edge wear.

There's be some fine swarf generated, so ideally you'd have a pan surrounding the vise and part, and use an aquarium pump for coolant application (don't grind dry), this would capture most of the swarf generated and keep if from the machine sump.

SigurdACVW · Mar 27, 2021

Hole size is slip-fit for 1/4" dowel, .2503".

Never heard of CBN pins. Interesting.

Each hole has 1/4" depth of 1/4" dowel and below that is 3/4" of 10-32 threads.

The design is that pins could be put into any of the holes as needed to accommodate any part or setup as needed. For example, two pins to line up a part with the machine axes, and one pin to stop it. No part will ever have to fit over all 50 at once.

Nagol · Mar 27, 2021

This is the same basic use case of my fixtures just bigger. Pin fixtures to each other when needed, use shoulder bolts for stops when needed. Bolt stuff down when clamping. Unless you are doing some crazy tolerance stuff the alignment you get from milling it should be good enough in my opinion. should be within a tenth or 2 if indicated in well when machining.

plastikdreams · Mar 27, 2021

If I were going to use an end mill I would use the largest od I could get with at least 5 flutes and probably a .03 corner radius. As much rpms that you can muster and a very tight slow helix down. Possibly use one for roughing and one for finish, though the finish might be better done as a full depth pass. The fact that you are only removing 5k per side might lead me to do full depth for the rough as well.

wesg · Mar 27, 2021

I'd look at plunging them with a 1/4" 4ft with a corner radius. It will probably be a thou or more undersize. Theres a possibility a 10-32 shoulder screw would fit ok. They're usually a bit under. If so, turn the heads down. Hard to find, I think, hardened. I've usually seen them in 303.

implmex · Mar 27, 2021

Hi sigurdACVW:
I'm with plastikdreams when he recommends the biggest cutter you can stuff down the hole and still interpolate.
You could get a 6 mm 4 flute in there, or if you want a bigger interpolation circle and more room for the chips use a 5 mm.

I'm also with Nagol when he recommends not helixing it down the hole, but rather dropping right down to depth and circle interpolating out.

Set up a rougher and a separate finisher.
Rough to within 0.001" on the desired diameter, comping out as needed with each hole until a 0.249 gauge pin will just go in.

Switch to your finishing cutter, reset the comp a tenth at a time and kiss them all until your desired dowel will slide in.

Write your code so you can run each hole individually, and you can cut, measure, reset comp, cut again, measure again etc etc on one hole at a time.
You don't want to cycle through all the holes then reset the comp and cycle through them all again or you'll end up with loose holes and tight holes

If you rough them all first, and then finish them all with a new cutter you can get them each to a nice sliding fit if you're patient and don't mind playing with the comp as the finishing cutter begins to wear.
You can even run three cutters in succession if you're super anal and want it the very best it can be.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Nagol · Mar 27, 2021

I disagree with using the biggest tool you can fit in there. The closer you are to your hole size it can kind of multiply your feedrate. If you use a .236 endmill the tool path diameter will only be .014 making the circumference of your tool path 0.044. The machine is moving based on the CL of the tool so when your tool is traveling .044 and the cutting edge is traveling 0.785 it will multiply your feedrate a bunch. There is chip thinning out at the edge of the too but if you base it on speed factor calculations most companies recommend only to 2X the feed rate for light cuts, not 17X. If you use a tool 1/2 the diameter of the hole this gets much better and only roughly doubles the desired feedrate. Guhring recommends no less than 1.7X the D of the tool when doing helical interpolation and I believe this is why. I came up with these theories on my own but it proves out in the real world. Its easy to confirm based on how long it takes a tool to run. 3mm or 1/8" would be my tool choice here.

CarbideBob · Mar 27, 2021

Relived 1/8 endmill.
As cutting head as it were.
I'd also do the same with a grinding pin if that you like that method.
Full depth cutting length or grinding length will likely be a problem.
Bob

SigurdACVW · Mar 27, 2021

I appreciate all the suggestions. We don't have metric cutters, only 3/16. The occasional oddball 7/32 shows up. Marcus, with the full depth of cut, do you see the cutter pushing away in something that hard? I like the roughing, finishing and comping idea.

Milland · Mar 27, 2021

CarbideBob said:
Relived 1/8 endmill.
As cutting head as it were.
I'd also do the same with a grinding pin if that you like that method.
Full depth cutting length or grinding length will likely be a problem.
Bob

I agree with this - the grinding pin I pointed out is too long, and should be ground shorter on a diamond wheel. Or find one about 1/8" LOC.

What's interesting is the range in pin cost I've seen. More than 10 to 1 between some vendors. I have to guess that the cheaper pins are coming from China, but it's no guarantee that the more expensive ones aren't...

plastikdreams · Mar 28, 2021

It may be worth trying a solid carbide reamer...if it breaks you have the through hole to pound it out

I will say I'm kinda surprised at the choice of material for this mini pallet. Most that I have seen/made/used were aluminum.

Mike1974 · Mar 28, 2021

Nagol said:
I disagree with using the biggest tool you can fit in there. The closer you are to your hole size it can kind of multiply your feedrate. If you use a .236 endmill the tool path diameter will only be .014 making the circumference of your tool path 0.044. The machine is moving based on the CL of the tool so when your tool is traveling .044 and the cutting edge is traveling 0.785 it will multiply your feedrate a bunch. There is chip thinning out at the edge of the too but if you base it on speed factor calculations most companies recommend only to 2X the feed rate for light cuts, not 17X. If you use a tool 1/2 the diameter of the hole this gets much better and only roughly doubles the desired feedrate. Guhring recommends no less than 1.7X the D of the tool when doing helical interpolation and I believe this is why. I came up with these theories on my own but it proves out in the real world. Its easy to confirm based on how long it takes a tool to run. 3mm or 1/8" would be my tool choice here.

That is why you adjust the feedrate to match the cutter diameter/final hole size. AND some machines/cam systems will do this "slow down on arc moves" etc. For example (not hardened, but 'regular' mats, if I was using an 1/8" EM to mill a .175 hole (helix, which we do alot), I might have the helix only be .005/.01" rev, same tool doing a .260 hole, might have the path be .02-.03" rev. Adjusting feedrate as well accordingly.

I would probably use a 3/16" EM in OP case, full depth, circle mill, not helix bore, and run a finisher as suggested for final size.. I didn't see a RC, or I missed it, but up to 54-56 should cut just fine with a regular carbide TiCn, ALTin, Firex, etc coating. ABove 56 might need to look into something specialised for the purpose.

13engines · Mar 28, 2021

If there's not one already, mill, not drill a 45 degree chamfer and chamfer all the holes. Then helical mill at depth once or twice around to to bring the hole closer to finished size and also re-establish some sense of location that has certainly been lost in heat treat. Then ream to size with a MA FORD Truesize carbide reamer, which will also appreciate that chamfer being there.

SigurdACVW · Mar 28, 2021

Hardness will be 58-60 C.

With the CBN grinding pins, is that a helix path or full depth comping out a little at a time? Are those cutters made to be a true cylinder?

Thanks for all the suggestions. I think my first attempt will be to try interpolating to .249 with an end mill and see the results.

CarbideBob · Mar 28, 2021

SigurdACVW said:
...
With the CBN grinding pins, .... Are those cutters made to be a true cylinder?

Yes or within the .0002 plated product can be made.
But like an endmill the shank deflects making it a now tapered hole which gets worse as the tool dulls.
Hence the relived or low contact side length on either.
Everything bends under load. Reamers are bigger on the tip on purpose.
Bob

Any suggestions for helix boring hardened A2?

Aluminum

Diamond

Titanium

Aluminum

Aluminum

Attachments

Diamond

Aluminum

Aluminum

Diamond

Titanium

Diamond

Aluminum

Diamond

Aluminum

Diamond

Diamond

Diamond

Stainless

Aluminum

Diamond

Similar threads