What's new
What's new

Help needed with deep pocket. .625 wide x 2.5" deep in 4140 pre hard

jspivey

Aluminum
Joined
Nov 18, 2018
Location
Southern Illinois
Hello all,

Let me start off by saying that I don't have much experience with extra long reach tools, so any and all advice is appreciated.

I have 18 parts with a .625" wide by 2.125" long by 2.5" deep pocket in them. Just to add some fun, the pocket finishes with a .125 corner radius. No, the design cannot be changed. The material is 4140 pre hard.

My first attempt at these pockets was using an Iscar ECI-4500-2.5COVF4. (1/2 endmill, 2.5LOC .015 corner radius). I've broken two of these endmills at this point and don't have any more on hand, or anything else long enough to try. On the second one, I had the chatter down quite a bit, but the endmill gave up not long into the pocket. Additionally, I realize that best case scenario is to rough out the pocket in steps with increasingly long endmills, however, that doesn't do me any good if I can't get the longest required EM to work. After roughing, I plan on going back in with a .25 endmill to finish the corners.

Toolpath was 3D adaptive clearing posted from Fusion 360.
Machine is a Dalian VDL-1000. CAT40, 8000 rpm spindle. No thru spindle coolant. Seems to be a good machine overall.

Cutting parameters when the second EM broke:
YG set screw holder. Relatively short gauge length.
Axial DOC: .25"
Radial DOC: .03"
Feed: .0015 IPT
Speed: 250 SFM (tried higher but chatter was terrible)
Entry method: 1/2" pre drilled hole

If currently waiting to hear back from the Iscar rep for our area to see what he can come up with.

I'd appreciate hearing what everybody's thoughts are as far as speeds, feeds, etc are. Thanks in advance.
 
Drill out as much material as possible with standard twist drills. Otherwise, look at sinker edm.
 
I'm starting with three .5 drilled holes. Should I start with one .5 hole to plunge into and try to drill out more with, say, a 1/4 drill? I can't see that it would make a ton of difference. I'm still going to have to fight chatter at some point.
 
Drill 4 .250 holes in the corners. Then drill a hole just over .500 in the center, get an endmill with corner radius on them. Then plunge mill from the hole outwards. Then take some cleanup cuts. Finish with a nice long .250 endmill spiraling down.
 
If it has to be milled you really should use a horizontal. Chip evacuation will be a problem no matter what you do. Loose chips will wreck lots of end mills. Stop after every Z pass and clean the pocket.

I believe I would drill out everything I could, including quarter inch holes on the corners. Then knock down the interstices with about a .610 custom spot face.
 
You need a short flute length necked cutter. I like the ones Helical sells. I have several 1/2" endmills that can reach 3" no prob. A pock ramp toolpath usually works well.
 
Ghuring Diver series may be a good option here. Very good at plunging and they have off the shelf options with through the tool coolant. Remove most of the material with plunge milling, That far of a reach your tool is only strong 1 direction.. towards the spindle. As far as finishing a good variable geometry endmill of any brand will help you not chatter. May also need to see if you can add RPM oscillation to combat chatter. In Summary, I would, Drill about .61 on both ends, Plunge down the center of the pocket, rough mill bigger( possibly with 2 different tools, 1 normal flute length, 1 neck relieved), Then finish when there is almost nothing left( probably a second pass on the finisher to ensure minimal taper and proper size.)

You didn't mention a tolerance on the slot.. pretty relevant.
 
Ghuring Diver series may be a good option here. Very good at plunging and they have off the shelf options with through the tool coolant. Remove most of the material with plunge milling, That far of a reach your tool is only strong 1 direction.. towards the spindle. As far as finishing a good variable geometry endmill of any brand will help you not chatter. May also need to see if you can add RPM oscillation to combat chatter. In Summary, I would, Drill about .61 on both ends, Plunge down the center of the pocket, rough mill bigger( possibly with 2 different tools, 1 normal flute length, 1 neck relieved), Then finish when there is almost nothing left( probably a second pass on the finisher to ensure minimal taper and proper size.)

You didn't mention a tolerance on the slot.. pretty relevant.

Tolerance on the slot is not tight. There is .01" clearance between the nominal finished slot dimensions and the mating part. I plan on trying to hold +.001 -.002 for later fixturing purposes. Nothing on these parts is very tight. The machine this will be done on has a Fanuc Oi- Mate-MD control, and I do not believe it supports RPM oscillation, but please correct me if I am wrong.

It sounds like plunge milling is going to be my best option. What kind of step over between plunges sounds realistic? Speeds and Feeds? No experience plunge milling.
 
could you use a high feed mill to remove the bulk of the material and then come back and finish with a solid to create the radius on the bottom
 
If you can get away with a slight step I would recommend only holding your fixturing tolerance as deep as you need it. As far as step over I would say 25 to 33 percent of the cutter step over. Feeds and speeds I would say start at whatever the manufacturer recommends and go 50% speed and about 70% feed to account for your long reach. may need to single block throughout to blow chips out of the hole with no thru coolant or air available. If no code available to oscillate speed can always stand there and do it with spindle override, just bump it up and down 10-20 percent as needed to keep chatter out of the finish, Added benefit of going a touch smaller below your fixturing depth is it will decrease load on whatever tool if finishing the rest of it. Just may want to leave .001 to finish any marring out after the bottom is done.
 
If you can get away with a slight step I would recommend only holding your fixturing tolerance as deep as you need it. As far as step over I would say 25 to 33 percent of the cutter step over. Feeds and speeds I would say start at whatever the manufacturer recommends and go 50% speed and about 70% feed to account for your long reach. may need to single block throughout to blow chips out of the hole with no thru coolant or air available. If no code available to oscillate speed can always stand there and do it with spindle override, just bump it up and down 10-20 percent as needed to keep chatter out of the finish, Added benefit of going a touch smaller below your fixturing depth is it will decrease load on whatever tool if finishing the rest of it. Just may want to leave .001 to finish any marring out after the bottom is done.

Single block in a pocket with the tool in the cut is going to cause chatter and rubbing where the tool stops, this will cause excess wear.
 
If you can get away with a slight step I would recommend only holding your fixturing tolerance as deep as you need it. As far as step over I would say 25 to 33 percent of the cutter step over. Feeds and speeds I would say start at whatever the manufacturer recommends and go 50% speed and about 70% feed to account for your long reach. may need to single block throughout to blow chips out of the hole with no thru coolant or air available. If no code available to oscillate speed can always stand there and do it with spindle override, just bump it up and down 10-20 percent as needed to keep chatter out of the finish, Added benefit of going a touch smaller below your fixturing depth is it will decrease load on whatever tool if finishing the rest of it. Just may want to leave .001 to finish any marring out after the bottom is done.

Unfortunately the depth for the fixture is nearly the entire depth of the pocket. There are a pair of bolt holes through the pocket nearly at the bottom that will be used to bolt it to the fixture. I will try to upload a picture to hopefully show better what I am talking about.

I was thinking about starting at around 10% stepover and working up from there after seeing how the tool reacted rather than starting too aggressive. As far as the endmill that will be used for the plunging, I was thinking of using a 5 flute EM w/ .03 cr from the same Iscar line I mentioned above. Additionally, I have tools at home to add additional relief to the EM if needed. I'm looking at the Iscar catalogue and the shortest flute on an appropriately long endmill is .875. I was thinking relieve an additional .375 so that I've got .5 of flute length and clearance behind that. Add similar relief to the .25 finisher.

In response to some of the other suggestions above, I seriously doubt I would be able to convince my boss to invest in any of the multimaster-like systems. We rarely do jobs like this. In fact, this is the first time since I've been here (4 years) that we've had a job like this. Vast majority of the jobs we do have depths of significantly less that 1.5*D.

Deep Pocket.jpg - Google Drive
 
Single block in a pocket with the tool in the cut is going to cause chatter and rubbing where the tool stops, this will cause excess wear.

If doing a plunge cycle it will be in rapid on the way out of the hole. Turn rapid down and hit single block on the way out..

I don't think a 25 percent step over would break the tool and you'll have to judge which way to go. The face of an endmill is somewhat concave so a balance needs to be achieved where it isn't pushing the tool out of the cut too much or pulling it in too much. I would say you'll wear things out rather quickly at a 10 percent engagement. A 5 flute will probably work fine but be careful on the first couple of pecks and make sure the flutes are loading up. A tool I would recommend would be a Gorilla Mill 4 flute with neck relief. Probably best to use a sharp corner or 0.015 radius to not introduce too much deflection. Bigger radius may help the corner but will likely introduce a worse cutting condition.
 








 
Back
Top