Can I get some advice on milling off a hat.

[Jaxian]

So I have a piece, it's 6" x 7" x 5/8" made of 6061. It ends up with a 1/2" thick feature with a 1/8" hat on the bottom. Kind of rounded triangular shaped. I flip it over put it in a set of milled soft jaws and mill off the 1/8" hat revealing the finished triangular part.

The CAM spat out .040" max DOC and 2750rpm,40IPM. So it goes .005", .045", .085", .125". This is with an Iscar 2" octomill facemill, 4 flute.

This issue is I ran it once and it made ugly noises. It is deflecting the material. Then when it gets to depth and finally shears it off the leftover that was deflecting gets flung. Loud noise, not cool. The finished part looks fine but I did stop and break off one section at the thin front so the next tool wouldn't run into it.
The final part looks great but I can't have it flinging chunks around. Plus I don't want to sit there and break off the extra every time.

I am trying to reduce the machining time on this and it already takes 4 minutes. Maybe use a 1/2" endmill instead and just mill off the full 1/8" at once so it won't deflect as much. Or deeper passes on the facemill or ? Open to suggestions.

Photos of the beat up scraps. The other side looks nice and machined. They are .090" thick at some spots.

 

[pato]

On parts like that I will usually do a profile around the part leaving some stock on the OD at Z-.02 or something or if the hat is too big for that do an adaptive/dynamic toolpath for the OD at 90% stepover. With it being that thin you should be able to go at a high enough feedrate to not take much time. Then just take one rough face and a finish face with your facemill and be done.

 

[Jaxian]

Let me see if I understand what you are saying. So take like my 1/2" end mill and do a outside adaptive profile of the part to remove the majority of the material. So full 1/8" +.01" or so. Then just go over the remaining material with a facemill to bring it to size.

I wonder how aggressive I can get with that end mill at only 1/8" thick without it vibrating. The corners of the triangle as you can see are hanging pretty far out in space. Totally annoying that it takes 20 min of milling op 1 and $10 of material every time I want to test.

 

[Garwood]

Drop the 1/2 em down so it's just above the vise jaws and zip around staying about 10 thou away from the part. Then use your face mill.

Or just take it all off with the face mill? Does your machine have the beef or is it on the lighter side? I usually step down .200" per pass full width of cut with a 2.5" ripper mill at 6000 RPM/120 IPM and it reads under 25% load on my Kitamura.

 

[pato]

Let me see if I understand what you are saying. So take like my 1/2" end mill and do a outside adaptive profile of the part to remove the majority of the material. So full 1/8" +.01" or so. Then just go over the remaining material with a facemill to bring it to size.

I wonder how aggressive I can get with that end mill at only 1/8" thick without it vibrating. The corners of the triangle as you can see are hanging pretty far out in space. Totally annoying that it takes 20 min of milling op 1 and $10 of material every time I want to test.

Yeah, at least that has worked for me many times. Even if doing a profile around the part flings a small piece sometimes I have let it sometimes, although I have gotten them jammed in the chip auger before. Generally I would not be too concerned about chatter in aluminum that thin and would go 200-600ipm with some endmill I don't care too much about even if it does not sound amazing, but maybe you have more unsupported material than I have dealt with in the past?

 

[MaxPrairie]

Like others said, profile with endmill first. If it is flinging the grip stock, slow the feed right before they break off then speed up again. Edit the facemill cycle by hand, you have the XY moves already there...

 

[Jaxian]

Ok, thanks guys I have some good stuff to try tomorrow. The machine is a Doosan DNM5700 and this is in a Chick vise so rigidity and power shouldn't be an issue. I do the first side using Talon jaws and the unsupported 6" resonated like crazy and gave me horrible surface finishes. Made up some shop made wedges which solved all of that thankfully so just trying to get second side working as well. I am assuming if I do a standard adaptive on the gripstock/hat at maybe 50%? stepover with a 1/2" end mill that should only throw little chips. I wonder if a four flute would be better so I always have a flute in the cut so no chance for spring back. Hmmm

There is 1/8" high durometer rubber between material and wedges not shown.

 

[Job Shopper TN]

Definitely rough to the profile with an end mill, or saw the excess off prior to op2. Depends on how much cycle time you have during op1. Then you can face as normal. Facemills grabbing thin flaps like this can be a disaster for sure.

 

[daringwilliams]

Tab the part in profile as last step of Setup1, smack it out with a hammer, only have a few cleanup areas and a facemill will bust through it

Also as said before, do a 2D profile till you have removed the perimeter top hat, switch to facemill and bust it off real fast

 

[PegroProX440]

That wedge idea is pretty clever

 

[Jaxian]

That wedge idea is pretty clever

Thanks, I tried just stuffing things under the material first but it didn't dampen enough. Then I cut some old soft jaws at a 1/2° but over 7" that's still like 1/8" drop so it was only touching at the edges doing nothing. Then I tried stuffing a bunch in from either side which kind of worked but it was easy to jack up the material. Plus the sliding in against the rubber material was a bear. That stuff does not allow sliding and everything moved while I was doing it.

So I figured I needed something like a scissor jack that only applied upward pressure and just a bit of compression so make it hand tighten. Also I wanted it to end up as a solid path from the material to the bed of the vise so nothing that could flex. I am amazed at how well it worked. Sounds like it is sitting right on the vise bed.

 

[Vancbiker]

For production jobs, my policy was to never allow remnant chunks. Turn it all to chips. Dropping chunks into augers or conveyors too often leads to them getting damaged. Particularly so with the rotary drum type fines conveyor systems where the chunks can easily damage the drum screen.

 

[Jaxian]

Just to report on what I did and how it worked. Took a 1/2" 3 flute with only 5/8" LOC, figured the more rigid the better. Figured if the hat/gripstock was .125" I would set DOC at .135" so it wasn't too far under the edge. Left .020" radial on the main model so I didn't actually mess up the edge finish from op 1. Let it go at 10,000rpm and 100ipm. I whimped out on the stepover left it at 10%, .050".

Worked fantastic. Didn't ring or make any weird noises. Just a nice solid hum. Then used the facemill to do two .0625" on the remaining material to bring it to dimension. So final piece is perfect with no sketchiness in the process.

Only downside is it added like 3 minutes to the operation. Thinking I might move the crossover from .050" to ...075"? or .100"? Any thoughts as the point it will start to have issues?

Thanks for the input guys, that helped hugely.

 

[daringwilliams]

I don't want to tell you how to program, but 40% stepover @ nearly 3x feed @ that depth would probably work just fine, and be MUCH faster with nearly 5.8 Ci MRR vs .7 Ci MRR

1/2" endmill in 6061 with a rigid setup good tool will eat that up all day

 

[Jaxian]

I don't want to tell you how to program, but 40% stepover @ nearly 3x feed @ that depth would probably work just fine, and be MUCH faster with nearly 5.8 Ci MRR vs .7 Ci MRR

1/2" endmill in 6061 with a rigid setup good tool will eat that up all day

Feel free to comment. I am almost always working on very small quantities or things where I absolutely can NOT scrap the original piece as there is no replacement. So I am always going at the very low end of the cutting range since there is nothing to be gained from cutting a bit of time off one operation. This particular one will get repeated many times so trying to get a feel for speeding things up.

I was very worried about the material hanging out in space but apparently at 1/8" thick and my 10k/100ipm/.135"doc settings it was just fine. I am only at .0033" ipt so I think I could go from .050" to .100" stepover and see how that works.

 

[LOTT]

A course knuckle rougher will do a nice, fast job getting rid of the top hat, you can really crank up the speeds and step over, and the chips are more compact to boot.

 

[50BMG DUDE]

I'd easily run that at 40-50% step over taking only that little bit. If you have more RPM, use it. You should be able to turn that to chips right quick. If you are not using a Aluminum only cutter try the YG-1 ALU-Pwr 3 flute polished. they are my go to. All thou I have had great luck with the Accupro 3 Flute ZrCN as well.

 

[implmex]

Hi jaxian:
I'm with Job Shopper TN in post #8.
I saw the flappy parts off with the upright bandsaw leaving 1/8" or so around the profile.
It takes seconds.

I can then Adaptive Rough or Facemill off the remainder (depending on how well the part is clamped for OP 2) after I profile around the part periphery first; climb cutting so I don't raise a bur around the edges of the finished part.
The extra time it takes to do that is worth it unless I plan to run a chamfer mill around the outside after facing it.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[Booze Daily]

Something I haven’t seen mentioned yet that I do sometimes.

Start at the exit side of your cut and take it within .010 or so of finish. Mill far enough to cover the width of your part. Then start at the other side to finish your thickness.

I do this on plastic and phenolic where the corners on the exit side are prone to chipping out.

May or may not work for your application but it’s an easy edit at the machine and shouldn’t add much to your cycle time.

 

[JSL_MFG]

If you helix down around the part before facing it, leave maybe .02 of radial stock on your part so you don't gouge it, you'll change the direction of cutting forces. This will usually allow you to mill it away without having a massive amount of vibration. I cut parts like this every day, and I always helix down around the "top hat" left over from op1 for this exact reason.