What's new
What's new

Deep hole grinding

M. Roberts

Cast Iron
Joined
May 11, 2021
Hello all. Its been a while since I have been on, hope all is well. I am working on a project that I am looking for a little advise on. The material is silicon carbide based ceramic, 0.625" thick. The task is to open up pre-existing holes from 0.285" diameter to a final dimension of 0.315" +/-0.001". My current process is as follows, one single 80 grit diamond abrasive tool per hole (a dedicated rougher per hole), and a common, 220g diamond abrasive tool per hole to finish all holes. I am taking the full depth of the part, 0.625", in a single pass, and stepping out in 0.0001" increments, leaving 0.001" for the 220g to take it to finish size. That is in 0.0001" increments, full depth. The machine is a Yasda 640 with a 24k spindle, running Rego Power Grip tool holders, at 20K RPM., 10IPM, flood coolant. The problem is that I am seeing some taper from top to bottom of the hole...cant exactly figure out why, and how to fix the issue...any advise?

Thanks,
Mark
 
Buck,
Good morning. Perhaps it is that I haven't had my coffee yet, but I do not understand your reply...can you elaborate?
Thanks,
Mark
 
I think he didn't realize that you were trying to grind full length at once with no in/out of the hole travel. It would probably work better to use a narrower point and interpolate down through. If you are using a non-dressable point it may not be perfectly straight. How much taper are you getting, and in which direction?
 
Hello eKretz, Thank you for the reply. I was trying to avoid the "Christmas tree effect" of the hole, that one would expect to see if you stepped down thru the hole...the tool would definitely preferentially wear....a full depth cut should (famous last words) wear evenly. The holes are ending up bigger on top versus the bottom...more than the tools themselves are tapered...which themselves are tapered about 0.0001" per side....not bad. In addition, the spec is 32Ra, and I am getting around a 45 Ra with a 220 grit tool.
I had thought that I may have an issue with lack of coolant flush/flow...there are blind holes in the fixture...wonder if I should cut channels to allow the coolant/swarf to flow away....any additional thoughts?

Mark
 
A .25" diameter diamond pin run at 20,000 rpm has a surface speed of 1308 ft/min. The Yasda milling spindle is not a good choice for your grinding operation. You could double the surface speed with a air turbine spindle. These air spindles are intending for milling rather than grinding.


Could you provide more information on your diamond plated grinding pins. A short grinding length relative to diameter would reduce the side load on the pin and reduce deflection.

Is it possible to adjust the feed rate as position changes on the Z axis of the mill during the grind cycle to compensate for the bell mouth on the bore? This would be the equivalent of adjusting the tarry delays on a ID grinder.
 
Last edited:
If it's a blind hole, I wonder if you aren't hitting the bottom of the hole or rubbing in the bottom corner. That would flex the shank of the tool and might well create the taper that's smaller at the bottom. It might be easier to use a quick lap for final finishing.
 
Good morning. In the beginning of this project, the guys did try to use an air spindle, but there were issues. One of which was that the spindle didn't have enough torque...second, they were unable to execute a tool change due to the air line. The grinding pin/nib...0.250" carbide body...roughers 80 grit, finisher 220g. part is a nominal 0.625" thick; length of diamond abrasive is 0.700". I have the tools chuck up pretty far.

eKretz; no, the tool is not bottoming out; there is a decent chamfer on both sides of the hole, and there is a c-bore on the fixture to boot.
 
Good morning. In the beginning of this project, the guys did try to use an air spindle, but there were issues. One of which was that the spindle didn't have enough torque...second, they were unable to execute a tool change due to the air line. The grinding pin/nib...0.250" carbide body...roughers 80 grit, finisher 220g. part is a nominal 0.625" thick; length of diamond abrasive is 0.700". I have the tools chuck up pretty far.

eKretz; no, the tool is not bottoming out; there is a decent chamfer on both sides of the hole, and there is a c-bore on the fixture to boot.

I misunderstood. I thought you meant that the holes in the ceramic workpiece were blind. In reality, you meant that the exit side of the holes are covered by a small c'bore in the fixture. So yes, I would definitely cut exit holes for the coolant.

How did the taper look with the air spindle doing the work?
 
I think the op should show the tool. If a point mounted wheel on a carbide shank, and a through hole then coming out of the hole at one end or both can/will/may produce a taper or an hour glass shape bore. One common technique is to begin grinding in the hole, then travel in/out with the wheel not exiting the hole fully. The wheel might exit only 1/2 or 1/3 or what depending on the part.
For a blind hole one may need start grinding at the bottom and travel outward to 1/2 or 1/3 so to keep the wheel straight sided.
Problem can be the increased circle the wheel turns when it is not under load(grinding), or the grinding action causing the wheel to wear to hourglass shape or tapered.
A very fussy part might need a short travle, only coming 1/2 - 1/3 out of the part every other time.

A final dimension of 0.315" +/-0.001" seems a very doable size
 
Last edited:
Attached is the picture, somewhat staged. Shows the part, the tool in the holder with the typical projection.....
 

Attachments

  • yasda grind.jpg
    yasda grind.jpg
    914.9 KB · Views: 25
The grinding pin is being used as if it were in a router.
The bell mouth at the top of the bore implies that the grinding operation has not sparked out at the base of the bore. Does the bore taper decrease if you slow down the X-Y table oscillation to 1/2 or 1/4 of the current speed?
 
I find it difficult to believe that it's a tool pressure problem if he's only leaving .001" to finish grind. We also still haven't been told the actual amount of taper...

I would still try the move to a narrower pin and interpolate, myself. Run the pin down through and back up a few times and see if you get a straight hole. A Yasda is a pretty solid machine, and if that pin is solid carbide I don't think you'll be getting a lot of deflection with that small amount of stock.
 
Good morning. Thank you for all of the feedback. I am of the same mindset...the set-up is pretty solid...I do not think that deflection is the issue...but what is the root cause. And I am sad to say that I have not personally checked the parts, or ran the parts, but I had someone do it under my direction...I really should verify all the issues myself...100% my fault.
Mark
 
I think we need to know the actual amount of taper you're getting in the hole. Check the hole, then check the tool that was used for the finish and report back. Also, what is that toolholding setup? At first I thought that it was a shrink fit holder, but upon closer examination of the photo, it looks like there's a split bushing in there?
 
I find it difficult to believe that it's a tool pressure problem if he's only leaving .001" to finish grind. ........ I don't think you'll be getting a lot of deflection with that small amount of stock.

The grit density on the grinding pin is too low to insure a smooth surface without a pin Z axis oscillation. I suspect that the pin is rubbing on the workpiece between the gaps of the diamond grit. The wear band in the photo of the grinding pin suggests that the pin was held fixed in Z while grinding.
 
Last edited:
The grit density on the grinding pin is too low to insure a smooth surface without a pin Z axis oscillation. I suspect that the pin is rubbing on the workpiece between the gaps of the diamond grit. The wear band in the photo of the grinding pin suggests that the pin was held fixed in Z while grinding.

I don't think the photo is showing the finishing pin - that's a much lower grit than 220...

And he already mentioned grinding full width, with no in/out.
 
Good morning. On a path to confirm the taper and the surface finish of the holes. eKretz, thank you for repeating that there is no Z movement; I feel that if there was, it would produce a "bell mouth" on both the entry and exit of the hole. And the tool in the pic is of one of the 80grit tools...the pic was just to represent the process. When I started down this path, I really wanted a true grinding nib...a tool that actually has some depth/thickness to the abrasive layer...so it could possibly be trued and dressed. My hesitation was that the shank would be much smaller in diameter, thus weaker and/or more prone to flexing and breakage. I will post actual taper of the holes...
 
IMO you have way to much grinding abrasive in contact with the hole. Your pin is deflecting. Dress that so there is only about 3/16 to 1/4 of abrasive length in contact with the hole, then program it so the pin strokes the hole. Pull the abrasive out of the hole by about 1/3 of the abrasive length each end for starters, this number may need to be refined.
 








 
Back
Top