My current design job is a medical grade drill bit for bone.

I am new to drill bits. I did my research on the characteristics of the drill point, the many geometries available and the theory behind the angles and facets. But for Pete's sake, I can't find anything on the actual manufacturing of the bits.

What is the flute profile? I know it's the grinding wheel profile, but what is that? I want to include the correct profile in the solid model.

What is the toolpath? How does the wheel orient to the stock? How does it begin the cut? Radial feed in? Radial with axial advance? Begin the cut at the point or the shank?

I have the material for the bit specified as a 15-5 stainless, 45 HRC (15-5 h900).

Now I need a shop. Most of the big guys won't call me back (Kennametal owns Cleveland and Greenfield). The few I have talked to won't do stainless(Republic/Michigan). I have set up RFQs with some small shops, but no results yet.

Please help. If you know a shop or have some detail about the toolpath.

Are you looking for a shop to make these drill bits? or are you looking for someone to tell you how to do them? If you are looking for a shop to do them for you I work for a company whose main product group is medical drills and cutting tools. We are located in Michigan. If you wish for us to quote send me a PM and I will give you the email for our sales rep. About 99% of our parts are stainless steel. Our engineering group could even help you with your design if you wish. Here is our website if you wish to take a look.

http://www.precisionedge.com/main.html

Good luck!:)

What is the flute profile?

The flute profile is the shape of the flute, hold the drill in your hand (shank side in hand) & look straight at the drill point (see attached image below). In the photo the red line is the flute profile. It is not only the grinding wheel profile, I run a cnc toolgrinder (840D/5-axis) & I can make the radius in the photo with a 90deg. 1A1 wheel.



What is the toolpath?
The toolpath is the g-code. (what path will the wheel follow?)



How does the wheel orient to the stock? How does it begin the cut? Radial feed in? Radial with axial advance? Begin the cut at the point or the shank?
Depends on the wheel & the machine. Most cnc grinder controls (840D, etc..) manufactures have addon software that creates the toolpath, leadin, leadout, etc...

Example, on my machine I can start the flute profile from the point, or the shank side, & as many passes as I want.



.

(This is not meant to be a smart a$$ remark, :) )


If all your doing is the design of the drill, really it shouldn't matter to you how it's made.


Give the manufacture a print, that's all they should need.


.

Sorry, What I should have asked is:What path will the tool follow? Will the material turn about the "A" axis and the tool move along X? (thinking in a 4-Axis mill scenario here) I imagine the grinding wheel would maintain a constant relation to the axis of the material. This relation would be governed by the helical pitch of the flute. One "A-axis" revolution would coincide with one helical pitch.

And I know where the flute profile is. What is the wheel profile that matches? You can use a 1/4" endmill to do a lot of passes and create some complex geometries, but a .250 inside radius between the wall and floor of a pocket is a lot easier with a 1/2" ballnose endmill. So, I suspect, the same applies to drill flutes. There is probably a given size that coresponds to each drill diameter, and a depth of cut that creates a standard web thickness.

As I am creating the solid model, it helps to know the path. I treat solid modeling like machining(virtual machining?). My sketch profiles are like tool silhouettes and the extrusion path is like a tool path.

I want to understand the process. If I just randomly send out drawings, somebody may waste a lot of their time and my (company's) money following a drawing that should have been done differently. We see it at our shop when we take on contract jobs. Unspecified dimensions and unrealistic tolerances waste a lot of our time. I don't want to be the guy that causes those problems. If I can take some time to learn the limitations and advantages of the process, I can design to compliment the process.

So, that's why.

Oh, I understand what G-code is. I have some experience with NC mills. I took a few extra shop and NC classes as part of my ME degree.

The cnc I run is a 5-axis (X,Y,Z,A,C) Schutte W305 840D, I use all 5 axis to grind the flute.

This is how I grind a blank, with & without coolant holes (2 flute). The drill program I use is a proprietary software from Schutte, I enter all my wheel info before I start working on the drill flute, then I work from a print for the drill info.

1) Probe the face of the blank with a Renishaw probe (set the X=0.000, & any coolant holes)

2) Select the wheel from the wheel magazine, I use a 1A1 wheel with a 90deg. corner that is wider than the drill flute, need to be wider so it cleans everything up. I could use a 11V9 cup wheel, it's my choice I run the machine, end result is the same.

3) Rapid (G90) all 5-axis to zero, set (G91) for the actual grinding, the Z-axis is set to whatever depth I need the flute to be, the Y-axis is offset to the drill center, the C-axis is set to whatever lead I need, & stays fixed in that position.

4) The actual grinding starts, Infeed is in the X-axis, most times starting from the point side working my way towards the shank. The A-axis is also rotating.

5) Rapid out of the 1st flute, send all axis to 0.000 (G91), index the A-axis 180deg., & repeat just like the first flute.

6) Send all axis home (G90)




.

Almost all high end cnc fluting machines have proprietary software which acts somewhat like a conversational control. to get different grooves you can just put a profile on your wheel with a cnc wheel dresser. At my company we have about 10 or these:

http://www.rollomatic.ch/prod620main.php?mach=620

and some other smaller fluters that do simpler parts.

Almost all high end cnc fluting machines have proprietary software which acts somewhat like a conversational control. to get different grooves you can just put a profile on your wheel with a cnc wheel dresser. At my company we have about 10 or these:

http://www.rollomatic.ch/prod620main.php?mach=620

and some other smaller fluters that do simpler parts.

I just use a 90deg.1A1 wheel straight out of the box, then program the profile.


.

Though i can't specify wich keywords to use ,i'ld say try youtube and alikes.
I've seen quite some vids of manufacturing processes including mills and drills.
I don't hink you'll ever get a clearer picture then a vid.

Good luck.

Though i can't specify wich keywords to use ,i'ld say try youtube and alikes.
I've seen quite some vids of manufacturing processes including mills and drills.
I don't hink you'll ever get a clearer picture then a vid.
Good luck.

I agree.


.

Thanks all, Especially Switcher.

So Switcher, can you describe the transition from full z depth to no wheel contact?

Is it a z-axis feed[G91] as the x-axis continues at the original [g91] feed?
What is the relataion/ratio? (2ipm along x-axis to 1imp along the y-axis)

Is there any y-axis movement during the operation?

Does the c-axis change during one part. I can see that the c-value would be different depending on the lead angle (helical pitch). But that should be constant for my application. I have seen the variable angle endmills for cutting aluminum.

Thanks for your time. I really appreciate you sharing your expertise.

can you describe the transition from full z depth to no wheel contact?
If your asking about when the flute is finished, & the wheel exits the flute, I program a small amount of over travel (approx. 1.0mm) I would still be in G91, I also do the same before the wheel touches the drill (pre travel, approx. 1.0mm (G91)), so that the wheel isn't slamming into the drill, when it rapids up to the drill (G90).



What is the relataion/ratio? (2ipm along x-axis to 1imp along the y-axis)
I might have mislead you, when I said "I use all 5 axis to grind the flute", actually for a basic 2-flute drill the "Y,Z, & C-axis" are only used to Rapid (G90) up to the drill & then stay fixed in that position, the actual infeed (G91) is in only "X & A-axis"

I work in metric so the 2ipm converts to "50.80" that sounds correct for the "X & A-axis" feeds (G91).



Is there any y-axis movement during the operation?
No, after the "Y-axis" Rapids to the drill it stays fixed in that position, during the entire grinding process.


Does the c-axis change during one part.
No, just like the "Y, Z-axis" the "C-axis" Rapids to the drill and stays fixed in that position, during the entire grinding process.





NOTE:
Just like any other program everything depends on how the machine is setup, how many axis, etc...


.

This is the machine I use (WU305).

http://www.schuttetgm.com/305.htm




And the software.
http://www.schuttetgm.com/software.htm


.