EndMill Performance using Dynamic Tool Paths

[Tinyfxds]

I'm looking to shave some time off a production job and have been given the green light to research new tooling to do so.  One of the biggest questions I've always had was how much does the helix angle on the cutter affect the tools performance when using a dynamic tool path?  What angle would give you the all around best performance 30, 35, 40, or 45° ?  Any insights on the subject would be greatly appreciated. 

 

BTW - These parts are aluminum and will be running on 2 different machines.  one with 20000 RPM (okk) and another with 12000 RPM (Hurco)

 

[BenK]

I think this is a much deeper question than just angle. If you are looking to improve your roughing times look at the Benchmark Carbide R350 series. They are some of the best roughing tools I have seen.

[crazy^millman]

How fast do you want the chip to come out of the cut without reducing the strength of the edge? That is really what it comes down to the less the angle the stronger the edge and more than angle the weaker the edge is my thoughts on it. I am sure my dumb way of thinking will get blow all to pieces, but here is how I explain rake to people. Yes it applies here. Negative angle is to take a shovel and turn it backwards and drag in across the ground at a depth to remove the dirt. Neutral is to stand the shovel straight up and drag it across the dirt at a depth to remove the soil. Positive is to turn the shovel at some angle towards the dirt to remove the dirt. 2 of which are almost impossible to do with human strength. Now each ways will dig a hole, but which one you can you do? The greater the angle to me from Horizontal is the less positive of a cut and the more closer to horizontal is more positive of a cut. The helix angle is that actin along the edge of the endmill as it is cutting through the material. Each angle has different benefits depending on the cut, machine, setup, speed, depth and many other factors. I tell people learning to only way to learn is to do it. Don't read about it don't just research it, but get out there and do it. That is the root of all learning not a bunch those stupid theories, but actual facts.

 

Buy several different endmills and try many different things. Record the results and put them through a series of tests and see how and what each one does. Measure the chip thickness and look at the edge under a microscope. The smell of the material and the sounds tell a story listen and observe them. Look at your load meter and push it and see how your machine reacts to different cuts. Bosses will argue you don't have that kind of time. They have no clue how to run the business then. HST is a game changing process and mind set and the idea of we have always done it that ways needs to be run over with a Mack truck. Tell that boss to allow you to do your job and be effective at it. Tell him to empower you to make money not throw it away.

 

If your boss(es) is(are)  the reasonable type(s) that understand yes it does take money to make it. If they understand you need sometimes to sort this out and get the facts to prove what you got is the best way or that you can improve it to make more money then Amen. If not then you must decide if you want to be part of the group that embraces change and wants to see things improve or are you happy with how it is.

 

Many things to consider and might talk to a couple different tool reps and have them come in and work with you and allow them the information. You do that and they will work with you. Tell them to send you free stuff and never work with them and forget about them helping you. We need to help each other and part of that is doing what you just did. Ask a question or many questions. I for one and glad to see you ask shows me a great deal about your character. You are not over in OT berating others you are learning so I applaud you for that. I have been doing this for 30 years and I pray I keep doing what you are doing. I have been doing it and that is ask question even if others may think they are stupid. I am humble enough to say if there a better way? Can I do this better? Can i Learn something from this or that person? I don't have all the answers sure which I did, but what  know I know and I know because I did it and I learned it and no one I mean no one can take that away from me or you. I don't look back and regret the long hours of learning and trying and not getting paid for it or getting called names or almost beat up because I was trying to better myself. Now people respect what I have to say and I hope it is always because I don't ask for it is because I give it. 

 

Sorry to throw my .01 cents into it, but keep on keep on.

[jeff]

For aluminum, I love the 3 flute, 45 deg helix.  Either bright polish or ZrN coating.

The 45 deg allows for good chip evac in slots, as it tends to shoot the chips up and out of the part.

Have a look at OSG Aero Blizzard. 

I used to buy mine from Lakeshore Carbide, but it seems they stopped making them. 

http://www.osgtool.com/_branding/books/8002014ca/8002014ca.html?pn=596

[Tinyfxds]

We have used a Walters endmill with some pretty good results.  I believe the angle on that is 40° and the Garr Alumastar endmills have a 38° angle.  I will start with these two endmills and give it a try.  Neither one of the tool reps for these two tools really understand how to apply the dynamic tool paths to the cutters they have.  I showed them the tool paths and explained what it's doing but they both cant seem to comprehend the large depth of cut but relatively small step over percentage.  They keep leaning towards small depth of cuts with big step overs. 

[Newbeeee™]

We run MAFord 134's at 150% LOC, 30% stepover, S10000, F7500mm/min (dynamic).

Bob W runs 200% LOC, 30% stepover, S14000, F10000mm/min. The tools are great.

We run the Garr fine pitch ally roughers on some thin wall parts and also some really deep parts because being fine pitch, there's less for the finisher to do.

 

Ultimately if you toolpath a typical job as per normal, then throw a path on it with the above settings, and look at the estimates cycle time (backplot or post and NCPlot/Cimco).

You can see what best fits the shape of your jobs because sometimes old school is better (but only sometimes IMO).

[#Rekd™]

We use the Niagara A345 3 flute cutters, 45deg with TiCN coating.

[MIL-TFP-41]

Thing that drives me nuts with guys using dynamic paths in Alum is they plug in something like a 10% stepover as they would on steel. Unless you are dealing with thin walls or other factors 25% would be my minimum stepover.

 

For tools I really like the Garr Alumistar and Kennametal's AADE series.

 

5/8 tool, 25% stepover, 1" DOC, 18000 RPM, 420 IPM puts the load meter on our MAM right about 125%. Fills up a barrel very nicely.

[AMCNitro]

Ive had  good experience with the Helical, cant really give you a model number or name though.  3 flutes

[AMCNitro]

Thing that drives me nuts with guys using dynamic paths in Alum is they plug in something like a 10% stepover as they would on steel. Unless you are dealing with thin walls or other factors 25% would be my minimum stepover.

Yep!! Ive gone as far as .125 stepover and 1.5 DOC at like 300IPM, I like to stay at 250IPM unless its really high volume.

[Hardmill]

Install the trial of Gwizard nitro

Really good and showing you what goes on by tweaking different parameters

 

Just be sure to input all the correct data

We used it at one point to see how it stood next to Mastercam and SolidCam for speeds and feeds and the result were very good

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

PEACE
 

[Matthew Hajicek - Singularity]

HSMAdvisor and the Helical Milling Advisor are useful too:

 

http://hsmadvisor.com/

 

http://www.1helical.com/index.php/milling-advisor

[guitar]

I would use Swiftcarb Ramp mill AV3 end mills in aluminum.

[guitar]

HSMAdvisor and the Helical Milling Advisor are useful too:

 

http://hsmadvisor.com/

 

http://www.1helical.com/index.php/milling-advisor

 

 

The new version of milling advisor requires internet connection. The older versions do not.

[Mike@Lustre]

we run Harvey Tooling on our ROBO DRILL using Volumill and have had really good success with tool life , smallest cutter is either .012" or .015" .

[bd41612]

I used to run Garr 41983's as my all around aluminum utility endmill.  100% axial 50% radial 14000 rpm 200ipm with no dynamic paths.  And they were in endmill holders, sticking out over 2".  I would change them out at about 10000 minutes of cut time.  Dynamic paths are awesome on difficult materials, but for aluminum I haven't tried it yet.

[jas6142]

I would say go with helical. The tech can actually use mastercam and put a  dynamic toolpath on it if your not sure of the parameters.

[tim_h]

If only I could keep the operators from backing down the feeds to 20 ipm...

 

   

[jeff]

If only I could keep the operators from backing down the feeds to 20 ipm...

 

   

On my Okuma I had an operator that liked to mess with the overrides. He ran 2nd shift on a couple of production jobs, and I kept wondering why his part count was so low.

After I locked out the override switches with M codes in the program, his part count soared.  

[Bob W.]

On my Okuma I had an operator that liked to mess with the overrides. He ran 2nd shift on a couple of production jobs, and I kept wondering why his part count was so low.

After I locked out the override switches with M codes in the program, his part count soared.  

Hey, but he has better spindle utilization (fewer cycles = less down time due to part change out) with half the effort. 

[Bob W.]

I don't know why shops keep these expensive guys around.  If you drop the feeds by 20% you just dropped the machine's productivity by 20% and that is EXPENSIVE!  Just as expensive as the guy that lets the machine run at 100% but then lets it sit for 25 minutes between cycles on a two hour part.  Makes a Makino as productive as a Haas...

[Matthew Hajicek - Singularity]

Hey, but he has better spindle utilization (fewer cycles = less down time due to part change out) with half the effort. 

 

That's the problem with metrics like that.