O/T Small Groove

[shienh]

I need to machine .032 wide .04 deep grooves on aluminum plate. Total linear length of grooves is 1800". I'm limited with RPM to max 10000.

 

Any one have any suggestions for cutter. I've to do this part on H. Boring mill.

[Nominal]

Not knowing what your part looks like, can you use an arbor mounted slitting saw?

[chris m]

Check this link:

 

http://www.robbjack.com/pdf/std_pg9.pdf

 

Robb Jack endmills are sweeeeeeet; the surface speed is REALLY low at 10K but carbide is probably all you're gonna find that small

 

C

[shienh]

I can't use slitting saw.

I'm using HSS endmill. .005 depth of cut but it is taking forever at 5.00" feed.

I will check robbjack

[Mike Whitten CAD/CAM Contractors]

shienh,

 

You should be able to go much faster that that. Make sure that the flute length on the em is not more than needed. Have them modified to .040loc if you must. I would take 2 or 3 passes in depth and also do a test and purposely blow up a few em's on a piece of scrap to see how fast I could go.

 

Mike

[shienh]

Michael

 

I tried different combinations of depth of cut and feed. At this feed it lasts for couple hours. More then this they are breaking every 15 min to 1/2 hour.

 

Chris

 

I did take look at robbjack tuffy endmills they do have one with 040 dia and .060 flute length. I will give it a try on Monday.

[Mike Whitten CAD/CAM Contractors]

Chris,

 

quote:

---

I did take look at robbjack tuffy endmills they do have one with 040 dia and .060 flute length. I will give it a try on Monday.

---

I agree with this as tool wear will not be your problem anymore.

 

Mike

[Mike Whitten CAD/CAM Contractors]

I still think the feedrate / depth of cut seems a bit slow. Look at reducing the flute length.

 

Mike

[Rob Dusenbury CAD/CAM CONSULTING]

Use pocket and turn on High speed cutting method, with "troicoidial cuts" I know the spelling is wrong but you should find it. Adjust the loop cuts and that tool will never be buried into the matl. You should be able to fly through that slot at a faster feed rate with the spindle speed max.

[Mike Whitten CAD/CAM Contractors]

Rob,

 

That sound cool but have you had good luck with this path, speed wise? It seems to slow things down instead of speed things up. I must admit I have never tried it on the machine though. I was thinking it was just for hardened material.

 

Mike

[Chris Rizzo]

Sounds like the hss tool is dulling after 15 min, and then rubbing, and then breaking. A carbide e.m , especially a top-quality one from Robb-Jack, will hold an edge much, much, longer. Probably use 2-3 on the 1000".

 

Rob,

 

you've had good luck with that trochoidal feature? I've had it make the cut time 2x-3x longer than reg. pocket. Because the tool is always taking light cuts, are you supposed to be able to crank the feed up to compensate for the extended travel distance incurred by all the little arcs?

[Rob Dusenbury CAD/CAM CONSULTING]

Crank the feed rates up and it should cut the whole length without breaking. Yes it will cut longer because of more feed motion but at faster rates it will all even out. This tool path will keep the tool from being burried into the matl. The way you are cutting it now keeps the tool burried into the matl the whole time that is why the tool is breaking.

 

Also another thought you might want to stick a lathe bit in or somthing simular the same thickness or smaller as the slot and broach it. Not sure what kind of matl your cutting but I have done this too.

[Mike Whitten CAD/CAM Contractors]

Rob,

 

quote:

---

Also another thought you might want to stick a lathe bit in or somthing simular the same thickness or smaller as the slot and broach it. Not sure what kind of matl your cutting but I have done this too.

---

Cool! Thats a good one Rob! I never thought of that but you could through a grove tool in the holder at the proper orientation and take cuts just like a Lathe.

 

Thanks,

 

Mike

[Midwest]

I cut ribs into steel with small carbide cutters @ 10,0000 rpm's with a feed rate of 100 ipm and a depth of .0005 per pass with really good results. They also have draft on the sides. I have been cutting alot deeper than .040 deep. (.500-.750 deep) using this method.

 

Crank up the rpm's and feed and blow a good steam of air at it and go do something else.

 

Aluminum may do better with coolant.

[Midwest]

One more thing, when cutting steel, you will get a ton of little needles (small chips) in your hands if you are not careful.

 

[iowajim62]

Midwest,

 

quote:

---

One more thing, when cutting steel, you will get a ton of little needles (small chips) in your hands if you are not careful

---

Ever try setting magnets around the part your cutting and getting the "needles" stuck there instead ? just a thought...

[MetalMarvels]

quote:

---

Ever try setting magnets around the part your cutting and getting the "needles" stuck there instead ? just a thought...

---

Great Idea! I tried it this morning and it really worked pretty good - stuck some disc-type ceramic magnets along the toolpath and I think it grabbed most of the "needles". Pulling the magnets off was fun though - miniature porcupines. Wish it worked for stainless.

[Frank]

I use the rob Jack cutters all the time for engraving cam covers or putting "O" ring grooves in blocks. Put your spindle at 7000 rpm's and run at 15. ipm and go for the full cut you should be fine.

 

Frank