What's new
What's new

Simple Slot Survey

Nerdlinger

Stainless
Joined
Aug 10, 2013
Location
Chicago, IL
Hi Everybody! I need to cut a .568” wide slot .895” deep through a block of annealed 4140. The slot is .875” long because that’s how wide the part is. It is rigidly held with serrated pads on a hydraulic vice with ten billion pounds of clamping force. The part is sticking up about 1.2” out of the vice.

Machine is a dual contact Speedio S700.

I am considering three ways to do this.

1. Full slot with 1/2” end mill right down the center, leaving about .034” on each side for a finish pass. (Or maybe a semi-finish pass that leaves .005” on the walls/floor for a real finish pass.). The only thing here is I’m not sure how deep I can go on each pass with 1/2” em on the 30 taper…maybe .375”?

2. Same as above but with a 14.5mm end mill and thusly leave nothing on the walls for a finish pass. Same concern at #1 regarding machine rigidity, though.

3. Same as #1 but with a 3/8” end mill since the Brother might tolerate the smaller cutter a little better. Maybe not right down the center, though…so maybe left side of slot, then right side of slot, then down and repeat.

4. Trochoidal rough with the 3/8” at full depth, leaving .005” on walls/floor for finish pass.

This is for long term production reliability/tool life is important.

Thank you for any thoughts you have on those options or others!
 
On a manual mill when I have to cut deep slots I always run an undersize roughing mill through first.
By far the fastest way to remove material on a lower powered machine. I have no idea how a roughing
mill would work in a CNC application.

From a production perspective I suspect you'd be further ahead doing everything with a single endmill...
 
Will option 4 cause more wear on your machine? I am only asking due to the long term production aspect.

Personally, I would choose option 3 but pre-drill a start hole with a carbide drill due to the depth and tool life factors.
 
Drill a 0.531 hole. Drop in said hole with 3/8 endmill then trochoidal it with an air blast would be best. Leave 5 per side for finish and come in with new endmill for finish if you prefer. Once rough endmill starts sparking switch it out with finish endmill. Don’t run coolant on it. It will decrease tool life and push the chips back in the slot. If you end up having to do 2 steps because of chip evacuation big deal at least the tool wear will be more spread out rather than all on the corner. I would start at 6500rpm and 80-100ipm with .025-.030 step over and see how it looks. Probably slow the start spiral up to 50% feed.
 
You've said it's .875 long because that's how wide the part is, so there is no drilling involved and you're coming in an out of the material.

On a 30 taper, I would use Option 3 with a stubby 3/8.
Mill back and forth .150 stepdown for about the .450 depth, then a quick profile on both sides, leaving .005-ish.
Then mill back and forth again with the same .150 steps to finish minus some, quick profile again leaving .007-ish so there is no rub.
Then whip out the 1/2" finisher for the final cut.

My personal preference:
I never use the same tool for rough and finish
I always leave very little for the finisher, and do it uniformly
 
On a manual mill when I have to cut deep slots I always run an undersize roughing mill through first.
The corncob kind with a bunch of little teeth instead of one long flute ? I love them things, they work great. In nc machines, too. Especially in a case like this with a small-power machine and a cut all the way around the cutter.
 
I'd go with a 3/8 variable helix end mill to rough it complete.
Cheaper to replace than indexable tooling and in this scenario probably just as fast as a high feed mill.
I haven't had much luck with the smaller high feed mills to be honest, the inserts are so tiny they are fragile little bastards. But you can also get a solid carbide HFM and test it out.
 
Ok if it’s just a slot the full width of the part then use option 6. High feed endmill.

I was always under the impression those high feed mills are like fast face mills...shallow depth but fast feed. I like that the force goes down in Z but do you really think it is faster than going straight through with an end mill?

Pic of part for reference:

IMG_7450 2.jpg
 
I was always under the impression those high feed mills are like fast face mills...shallow depth but fast feed. I like that the force goes down in Z but do you really think it is faster than going straight through with an end mill?

Pic of part for reference:

View attachment 335834

Thank you for posting a picture of the part. This was not what I had in my mind. The high feed endmill would be a little faster, but I think you could blow that out quickly with a 3/8 or 10mm endmill (on an adaptive path) pretty quickly as well. Maybe 30-45 seconds plus finish pass.
 
I'd go with a 3/8 variable helix end mill to rough it complete.
Cheaper to replace than indexable tooling and in this scenario probably just as fast as a high feed mill.
I haven't had much luck with the smaller high feed mills to be honest, the inserts are so tiny they are fragile little bastards. But you can also get a solid carbide HFM and test it out.

Yeah, when I mentioned high feed I was talking solid carbide. I have some 3/8 I have used. I am sure if you get a tool rep in there he will give you some freebies of what he thinks would be fastest. The nice thing about the adaptive strategy is like what I mentioned before, once the rougher goes to shit use the finisher and always have at least 3 tools in that rotation so there is no down time swapping out endmills.
 
I would use a trochoidal/adaptive toolpath, at full depth, because it makes a really cool pattern on the floor :D.

Seriously though, adaptive/trochoidal will extend tool life, be soft on the machine, and have low risk of breakage.

Regards.

Mike
 
I know a shop that makes 1000s of parts almost identical to yours. The use a 3/8" 5 flute full depth with a high speed tool path. Start with a 5% stepover and go up from there.
 
What about plunge roughing? Just me but hard to beat honking through with a drill, followed by emill plunging and finishing.
 
Hi Nerdlinger:
Is there a compelling reason not to saw these with a full width saw?
If you have to put that cross bore in anyway, it looks kinda attractive to me.

Mind you, I have no idea how stout a Speedio is so this may be a hopeless approach if the machine can't take big side loads, and you don't have a bigger VMC to put it on.

If I had to do it standing up like that, I'd trochoidal mill it to full depth like some others have suggested.

But this part screams "lay me over sideways" at least to me.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
Trochoidal with that geometry will crawl, just because there's no space to do the accel/decel/accel/decel so whatever feed rate you program in, you won't get it.

Which spindle is it? The 16k is very different from the high torque 10k. On my non-dual-contact 16k, I would probably do three passes with a .375 variable flute to rough, semi-finish one pass on each side full depth, then switch tools to a .375 finisher.

But mine are the least stout of the spindle options. You might be able to do it in 2 passes with good results.

Trochoidal is great when you have some room to run between reversals, but it's so painful to watch on a narrow slot.
 
Trochoidal with that geometry will crawl, just because there's no space to do the accel/decel/accel/decel so whatever feed rate you program in, you won't get it.

Which spindle is it? The 16k is very different from the high torque 10k. On my non-dual-contact 16k, I would probably do three passes with a .375 variable flute to rough, semi-finish one pass on each side full depth, then switch tools to a .375 finisher.

But mine are the least stout of the spindle options. You might be able to do it in 2 passes with good results.

Trochoidal is great when you have some room to run between reversals, but it's so painful to watch on a narrow slot.

I would disagree with this. I think there is plenty of room to send a 3/8 in there. I don't have experience with a 30 taper, but it should be able to handle 20 thou step over. If it were on my machine I would start at 35 steps and 80 ipm and go from there. What CAM do you program on? Each one calculates trochoidal a bit differently.
 
Hi again Nerdlinger:
If these are for high volume production, how about having blanks waterjet cut (or laser cut?) from a heavy sheet so you don't have so much meat to remove in the milling.
Maybe a total non starter cost wise, but worth throwing out there to see how the costs for each approach stack up.

It looks like you're facing these things all over before you put in the slot anyway, so it's not like you'd have to do more handling with waterjet cut slugs...in fact you may end up handling them less because you don't need to saw them from a bar first...they come all ready for milling in a box from the waterjet vendor.
You'll certainly spend less on carbide, on coolant, and on chip management.

I'm not sure from just the picture, but it looks like you might even be able to nest them if you can get a small enough kerf from the waterjet so the blanks still clean up, but even if you can't, you might still be ahead.
As a last thought, do you think you could save enough handling to make it worthwhile, to start with a sheet that's been Blanchard ground to thickness so you don't have to process those two faces part by part?

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining
 
I use HSMworks inside Solidworks, but it isn't a limitation of the cam, it's a limitation of the machine. A speedio has really fast top speeds and really jaw-dropping z acceleration, but not so much in X and Y. Especially with the high accuracy modes turned on. Without them on, it blows corners pretty badly. You can program 80ipm all day for this move with a .375. the machine won't ever get close .

It's just a horses for courses thing. On a different machine it might work brilliantly.

I did think the suggestion to plunge mill it might yield some great results, though. That's using the best features of the machine (retract and repositioning speed) to maximum effect. This specific case is just such an awkward in-betweener. If it was deeper, plunge would be a no-brainer. If it was wider, trochoidal would be a slam dunk. If it was shallower, just blast through. IMHO.
 








 
Back
Top