What's new
What's new

Machining Strategy of a part: Advice/Second Set of Eyes Please

Johnny SolidWorks

Hot Rolled
Joined
Apr 2, 2013
Location
Rochester
Image 1.jpg

Looking at this print, material is CRS, tolerances are open, with the only really critical feature being the sharp corner called out by the asterisk.

The 1.07 and 0.85 dimensions are full radius slots, if that isn't clear, and the 0.85 horizontal dimension is to a small flat. The radii in the left hand view that aren't called out measure 0.140.

Since I have to finish these in the mill (Haas VMC) anyway, I had planned on doing the whole thing there, especially because I'm not super comfortable or confident with working those inside corners sharp on my manual lathe. I figured on doing the majority of the material removal with a straight EM, then coming back in with a reduced shank EM to do the .110 on a side undercut portion.

Is this more trouble than it's worth? Should I just suck it up and go for it on the lathe?

I'll have about 20 PCS to do at a time, maybe a hundred or so a year total, so I can probably make an undercut EM go a long way (assuming I can find the one I'm looking for - I haven't had any luck finding one that's got 1/8" on a side step out with a short enough flute length. I'm not crazy about grinding the shank down on a tool (because I'm not very good at it) but have skated by with it in the past.

Any other ideas or thoughts? Is there something stupid and simple that I'm missing?

Thanks
 
I’ve made bearing pullers before that looked just like that. All manual. Bored it out on the lathe, then layed it on its side in the mill. But now that I have a Cnc lathe and VMC, I would definitely do it there. Especially if you plan to make more than a couple.

Drill it out as big as you can, pocket mill to flatten out the bottom and open up the side, then (like Milland said) woodruff key cutter to get the under-cut
 
Already been said.. Key cutter, and done.. This aint rocket science.

If it was 1000's of them, and there was more material to remove, I might have
something custom made.. But at 100 a year, it would probably take 5 years to
recoup the cost...
 
I would at least get the majority of the material out on the Lathe. Do the Finishing and under-cut on the Mill. Using a Groove tool to do the Undercut on the Lathe isn't that big a deal, but on a Manual it can't compete.

R
 
You can use a 606 cutter (like this: McMaster-Carr), which is 3/16" wide and 3/4" OD. While you could go wider for fewer cuts (a 806), remember that you're cutting full width and near final diameter, so engagement is pretty high. These only have a ~9/32" stem connecting the cutting head to the shank, so you don't want to over stress them.

An extra minute cutting time could save you from breaking a cutter.
 
That is a dream part for a small, bar-fed cnc lathe, especially one with a C axis and live tooling! Finished parts drop off! :)

Personally... I would blank those on the engine lathe and finish them up on the Haas. But hey... that's just me. I'm definitely out-voted so far in the replies. :D


PM
 
One more little idea - use a stagger tooth key cutter to remove almost all the material in the undercut area. Cutting forces are lower. Then use a straight tooth with a little overlap to finish. Since only a few at a time a few extra seconds won't matter. :)
 
My default for a lot of this type of work recently has been to use a keyway cutter, but I'm doing a fair amount of this type of thing, and I'm really not having very good luck with them. I follow the manufacturer's feeds and speeds recommendations (Harvey, which I usually have very good luck with) but I seem to keep chipping corners off the teeth way faster than I should.

I honestly asked because I was starting to feel like I was over-using the tool type or method, and figured there was a better/smarter way. (A while back I asked a question about my struggles with an op I was doing with a slitting saw and was pointed towards a Harvey keyseat cutter, which is infinitely better than what I was doing before - which started the keyseat cutter kick I've been on.)

If this just is what it is, I'll have to figure out what I'm doing wrong with them, but there seems to be a strong consensus that this is the right approach.

Thanks all.
 
My default for a lot of this type of work recently has been to use a keyway cutter, but I'm doing a fair amount of this type of thing, and I'm really not having very good luck with them. I follow the manufacturer's feeds and speeds recommendations (Harvey, which I usually have very good luck with) but I seem to keep chipping corners off the teeth way faster than I should.

I honestly asked because I was starting to feel like I was over-using the tool type or method, and figured there was a better/smarter way. (A while back I asked a question about my struggles with an op I was doing with a slitting saw and was pointed towards a Harvey keyseat cutter, which is infinitely better than what I was doing before - which started the keyseat cutter kick I've been on.)

If this just is what it is, I'll have to figure out what I'm doing wrong with them, but there seems to be a strong consensus that this is the right approach.

Thanks all.

NO!!!! The right approach would be get a Turning Center, with at least a C-Axis, but Y is so much easier to program. It was said up a few posts, that would be a killer on a C-Axis Lathe.

R
 
If you're going to do these on the CNC mill, than honestly, the worst part might be blanking the parts out - facing the "bottom" side, as it will sit in your machine/vise.

The top-side work is pretty simple really. Endmill out the bulk of material, drill & tap the thru-hole, then finish the undercut with a key-seat cutter.




A C-axis/Y-axis lathe would certainly blow through these faster, but at (20) pcs./month I wouldn't bother with setting up the tools. Maybe if I could setup and run the entire year's 240pcs. at once.
 
A C-axis/Y-axis lathe would certainly blow through these faster, but at (20) pcs./month I wouldn't bother with setting up the tools. Maybe if I could setup and run the entire year's 240pcs. at once.

Maybe, I think it depends on how cute that undercut needs to be. The Drawing shows the undercut coming straight out from centerline of the part, but if a guy could fudge it just a little and only use a Groove bar to do it, without doing the fine Finishing with an Endmill, I would still use a lathe. 2.5 hours for the FAI. 15 minutes a part after that.

I mean there are 40? Tools loaded in the Machine, Endmills, Groove bars, Drills, Boring bars (not a Keyseat cutter). It's really just programming and switching jaws out. But hey, I would do everything on a Lathe if I could.


R
 
My default for a lot of this type of work recently has been to use a keyway cutter, but I'm doing a fair amount of this type of thing, and I'm really not having very good luck with them. I follow the manufacturer's feeds and speeds recommendations (Harvey, which I usually have very good luck with) but I seem to keep chipping corners off the teeth way faster than I should.

If this is happening, look at how stiff the setup is (flexing work or cutter holding will damage the tooling), too high a feedrate when engaging the work (using a keyseat cutter is like constantly milling into a corner), or bad chip evacuation due to poor coolant flow or fixturing.

I use these cutters pretty frequently and rarely have an issue, but then I tend to be cautious with S/F. Mild steel shouldn't be that bad to cut, but if you want to spend a little more, buy a carbide or carbide tipped cutter and ramp up the spindle speed to reduce chip load. Again, stiff fixturing and good chip removal matter.
 
I would start with 1.25" OD by 1.65" Length CRS round stock in the mill. Cut everything I could with 1/2" carbide EM. I don't much care for keyseat cutters (even though I use them all the time). If I need to remove real material with an undercut tool, I will grab a HSS or Carbide endmill and grind my relief. I think flat flutes or staggered flutes have way too much tool pressure and leave a shitty finish. I would get the top square corner with a keyseat and then remove all of the undercut material with a relieved 3/4" EM. They just cut so much better than a keyseat cutter and will be 10x more rigid.

Then I would make my lowest paid employee remove the back side of the material on a manual lathe.
 
Hi All:
I'm with the camp that believes the most efficient way is to turn the basic shape and then mill the two features that must be milled all on a live tooled lathe.
However, if it's going to have to be milled, I'm with G00 Proto regarding what cutters to use.
I find a necked down endmill to be miles more efficient than a keyseat or Woodruff or tee slot cutter.
Even if you have to pay someone like AB Tools to neck one down for you, you'll be tons faster in my experience and get a better result too.

So the strategy I'd use if I didn't have a lathe to do them:

Make the blanks double ended.
Stand them up 2 blanks at a time in soft jaws and drill them to get the meat out.
(With a carbide insert drill and HP through tool coolant, you can be almost as efficient as you can on the lathe to knock out the worst of it...a few seconds per part)
Mill the top step, then mill the undercut.
Cut them in half and face the ends.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
In our shop, I would probably turn the OD, drill the center hole and part in the lathe, toss in a soft jaw on the mill and HSM out the center. If I had a bunch to do I would finish the top of the undercut with a indexable grooving tool (iscar picoturn) and the bulk with a necked down endmill. For a couple; as other have said just a woodruff/ keyseat cutter.
 
I don't think anyone covered this but would you leave the part a whole cylindrical shape and used the keyseat cutter inside BEFORE trimming off one side? This would make a more rigid part while undercutting and keep the sf uniform throughout. Anyway that's what I think I would do. I'd not want any chatter towards the top of the undercut. I'd also have the local tool grinder relieve a standard em about .03 short. Cut down on the number of passed and actually cheaper than a keyseat cutter for me.
 
I don't think anyone covered this but would you leave the part a whole cylindrical shape and used the keyseat cutter inside BEFORE trimming off one side? This would make a more rigid part while undercutting and keep the sf uniform throughout. Anyway that's what I think I would do. I'd not want any chatter towards the top of the undercut. I'd also have the local tool grinder relieve a standard em about .03 short. Cut down on the number of passed and actually cheaper than a keyseat cutter for me.

I would mill the side off first to improve the coolant flow and chip evacuation. I would start at the top and work my way down using a key cutter so I left the most amount of material supporting the cut.
 
I would want to do this in one setup in my VMC

Tallish soft jaws, 2 bores, either to do bottom then top or two top ops

drill[thru with tap drill or bigger for mat'l removal]

interpolate with end mill .85

use a 3/4 with 1/2 shank end mill[used to have some decent OSG in this kicking around] interpolate undercut

countersink

rigid tap


Might have to grind the top of the flutes to get a nice square corner

I wouldn't want to involve 2 machines when one can do it
 








 
Back
Top