HSM In 17-4

[HateWhatOwnsYou]

I've done some HSM in 17-4 with generic cheap zcc Korean tooling, like others said before keep the chip load around .005 and your tool will be much happier.

 

My biggest issue was the tool packing up when it was rampin down in pockets so I started using coolant and .5deg ramp downs

[kunfuzed]

Is that actual chip thickness, meaning adjusting the feed rate based on RDOC?

[dstryr]

Destiny Tool 6 flute would be what I'd use.

I just cut a big (big for me) titanium part with them. 1/2" necked 2.250 .625 flute length .030 corner radius

100% Depth 5% stepover 300 sfm .005 IPT Cutter just mowed along. I had to cut a 3.750 bore 2.125 deep with only a pilot hole. Couldn't use a bigger tool because of wall thickness issues and since it was only 5 parts I didnt bother with using more than 1 tool to rough

 

 

I'd imagine you should be able to do that cut in 17-4 pretty easily

[HateWhatOwnsYou]

it is the theoretical chip thickness, but its not relative to the step over

 

feed rate divided by spindle speed divided by the number of flutes.

 

 

Is that actual chip thickness, meaning adjusting the feed rate based on RDOC?

[HateWhatOwnsYou]

Here's the feed and speed on another mold plate I was doing, material is 17-4 variant specifically for molds

 

1/2 CEM w/.06R

PHX SURPA

S7500 F150.0 DOC .750 SO .05

SPINDLE LOAD 25%

 

 

 

One other thing to take note of, if your took starts hitting holes in the plate that it doesn't know about and compensates for, it WILL ruin your tool.

 

I've also noticed the machine will play a big part of how the toolpath works, our haas is about as ringid as a Bridgeport with the quill unlocked.

[Newbeeee™]

Here's the feed and speed on another mold plate I was doing, material is 17-4 variant specifically for molds

 

1/2 CEM w/.06R

PHX SURPA

S7500 F150.0 DOC .750 SO .05

SPINDLE LOAD 25%

 

 

 

One other thing to take note of, if your took starts hitting holes in the plate that it doesn't know about and compensates for, it WILL ruin your tool.

 

I've also noticed the machine will play a big part of how the toolpath works, our haas is about as ringid as a Bridgeport with the quill unlocked.

That's good to know - thanks for posting.

I'd have thought the speed would have been around 5000rpm for that mtl.

[kunfuzed]

*UPDATE*

 

The Garr V5's I ordered came in!

 

I was going to put in Colin's numbers of 480sfm @ .0044 feed, but ended up using the HEM check box with a modified Iscar library tool (still Garr V5 at machine) and set it to the catalogue parameters, which ended up being close to Colin's numbers. Though the book said .0015 chip load, I went with .001 just to keep the feed manageable for the Haas, at a factor of 1.0 on the slider. Tool life seems good so far, and sounds much better to me!

 

 

Tool - 1/2" dia 1 1/4 loc x 2 1/4 reach

Toolpath - Dynamic OptiRough set to Iscar HEM

Speed/Feed - 400sfm @ .001 chip load. (4000rpm @ 138ipm)

Stepover/ Depth - 5% @ 1.5xD

[kunfuzed]

Five of those parts roughed, finally chipped a tooth. The others still looked pretty good though.

[jeff]

*UPDATE*

 

The Garr V5's I ordered came in!

 

I was going to put in Colin's numbers of 480sfm @ .0044 feed, but ended up using the HEM check box with a modified Iscar library tool (still Garr V5 at machine) and set it to the catalogue parameters, which ended up being close to Colin's numbers. Though the book said .0015 chip load, I went with .001 just to keep the feed manageable for the Haas, at a factor of 1.0 on the slider. Tool life seems good so far, and sounds much better to me!

 

 

Tool - 1/2" dia 1 1/4 loc x 2 1/4 reach

Toolpath - Dynamic OptiRough set to Iscar HEM

Speed/Feed - 400sfm @ .001 chip load. (4000rpm @ 138ipm)

Stepover/ Depth - 5% @ 1.5xD

 

What clamping system do you have on that rotary?

I'm looking for something like that for my Koma.

[Rstewart]

What clamping system do you have on that rotary?

I'm looking for something like that for my Koma.

Looks like the Techni Grip I have on our rotary.

[jeff]

Looks like the Techni Grip I have on our rotary.

Any idea of the price of something like that of that size?

[kunfuzed]

Yes, Technigrip. I'll try and see if anyone remembers what that cost, when I get in. I wanna say it's in the price range of a similarly sized Raptor. Homemade adapter to the face plate.

[dstryr]

Holy tool stick out.... lol

 

Mill the corners off that bad boy like this one

http://technigrip.com/products/3-75-5-axis-assembly/

[JoshC]

HSMAdvisor is the best for general purpose; I use it for my non-Helical brand cutters.  I like the Helical Milling Advisor for the Helical cutters because it has a complete and frequently updated library of all their cutters, and who should know their cutters best but them?  Sometimes I use both at once to get a second opinion sanity check.

 

+1 on that calc

I also really like the milling advisor made by 1helical for my Dynamic Motion cutting data. I have an older application of their calculator that is less specific to their tools so I use it for other brand tooling too and still find it gives me pretty accurate cutting data , the newest milling advisor is a bit more proprietary to their tools but for a free product or free calculator I think it is pretty awesome.  I used to use Gwizard from time to time but I like milling advisor better as you need less input data and even though it may have less features its all I need and works great. Just make sure to Select Volumill if you are doing dynamic as they don't have Dynamic listed but have it called volumill.

if anyone wants the calc I am referring to its 1helical.com and just look for milling advisor.

[civiceg]

I would like the old helical calculator, it was quick and simple and I no longer have it

[JoshC]

I would like the old helical calculator, it was quick and simple and I no longer have it

i did a quick upload to dropbox if you wan the old one. https://dl.dropboxusercontent.com/u/94415403/MillingAdvisorSetup-6.0-1982.exe

[civiceg]

Thanks man