Parameters for different materials

[Metals and materials]

Hello all, 

I am curious if anyone know of any good website where I can find good cutting parameters. Especially ""Depth of cut"" for different materials. I work with lot of different materials, I keep about 0.003 as average for cutting all materials except aluminum (I go like 0.007) but for 5 Axis machining, I want to be sure. 

Please advise me how to find the best parameters. I use machining doctors for speeds and feeds but it's hard to figure depth of cut for different materials. 

Thank you in advance!!

[JParis]

The tooling manufacturers numbers are always the best starting point of what a tool is capable of doing....

[crazy^millman]

HSMAdvisor is what I have used for many years.

[Newbeeee™]

3 thou and 7 thou DOC's?

So that's where the name "ever lasting carbide" comes from?

[Metals and materials]

Which sometimes is super slow. For 5 axis, I can go faster. Question, for me is, how much? 

[crazy^millman]

3 minutes ago, Metals and materials said:

Which sometimes is super slow. For 5 axis, I can go faster. Question, for me is, how much? 

SFM and Chip load per tooth are part of the equation. Setup, Holder and rigidity of the machine are other factors. I have run machines at 1200 ipm, 24,000 rpms removing 180 cubic inches a minute of material. I have run electrode machines at 45,000 rpms with a .01 ball endmill at 200 ipm. I have used 80,000 rpm speeders to run a .002 endmills in aluminum to do some engraving at 10 ipm. I have run 36" diameter 60 insert face mills at 4 ipm and 20 rpms. I have turned parts down to .003" in diameter up to 20 foot in diameter. The point is there is no one size fits all in the profession. You need to take so many factors into consideration hard to say how fat you can push your specific tool on your specific machine that that specific material at any given time. Why we ask for a Z2G most times to evaluate your situation and then make a guess.

[#Rekd™]

If you use Harvey tools and Helical Solutions (same parent company). They have an excellent Machining Advisor on their website, it is excellent.

I also use HSM advisor that Ron mentioned along with contacting the manufacturers for recommendations for step overs, depth of cuts and feed per tooth.

 

[JParis]

1 minute ago, #Rekd™ said:

If you use Harvey tools and Helical Solutions (same parent company). They have an excellent Machining Advisor on their website, it is excellent.

I also use HSM advisor that Ron mentioned along with contacting the manufacturers for recommendations for step overs, depth of cuts and feed per tooth.

 

 

28 minutes ago, crazy^millman said:

SFM and Chip load per tooth are part of the equation. Setup, Holder and rigidity of the machine are other factors. I have run machines at 1200 ipm, 24,000 rpms removing 180 cubic inches a minute of material. I have run electrode machines at 45,000 rpms with a .01 ball endmill at 200 ipm. I have used 80,000 rpm speeders to run a .002 endmills in aluminum to do some engraving at 10 ipm. I have run 36" diameter 60 insert face mills at 4 ipm and 20 rpms. I have turned parts down to .003" in diameter up to 20 foot in diameter. The point is there is no one size fits all in the profession. You need to take so many factors into consideration hard to say how fat you can push your specific tool on your specific machine that that specific material at any given time. Why we ask for a Z2G most times to evaluate your situation and then make a guess.

and through all of the good info here.....I'll reiterate, the set-up, rigidity, tooling and machine ALL come into play....use the starting numbers and adjust as is seen fit based on the feedback from the machine and results..

There really isn't a one size fits all answer here....many variables.

[cruzila]

OR....................run it till it blows up then back off 10%

[crazy^millman]

36 minutes ago, cruzila said:

OR....................run it till it blows up then back off 10%

Yes seems millions of dollars get lost using that principle over the years. I tell all customers running hard metals in a production setting to think of the 80% rule when it comes to running the tools. To many think they need to get that last 20% out of a tool and then it breaks scraps a part and they end up loosing up 100X the cost of the tool trying to cheap out getting that extra 20% out.

[Metals and materials]

A lot goes in calculating few parameters!!! I will start with manufacturer's numbers and move forward from there.

Just curious if anyone know, how do manufacturers come up with numbers? Do they just go till the tool blow up and take average or something?

[crazy^millman]

27 minutes ago, Metals and materials said:

A lot goes in calculating few parameters!!! I will start with manufacturer's numbers and move forward from there.

Just curious if anyone know, how do manufacturers come up with numbers? Do they just go till the tool blow up and take average or something?

LOLOL sorry I had to laugh when I read that, but yes that is part of their testing. Read up on perfect heat zone for coatings and materials. The real science that goes into coatings and other things is something I geek out on.

[Jobnt]

5 hours ago, cruzila said:

OR....................run it till it blows up then back off 10%

^^^ Tried and true method with decades of success for any material type!  

Axial engagement will vary depending on radial engagement. Try different combinations to find what works best.

You can run full depth with > 75% radial engagement but your feed will be very slow.

Or you can run full depth with < 10% radial engagement and extreme feed rates.

Or you can run at < 5% axial depth with full radial engagement and feed stupid-fast but I've never gotten the MRR to be more efficient using the last method. Machines usually can't accel fast enough to hit those kinds of feed rates before it has to slow down for the next corner.

[cruzila]

2 hours ago, Metals and materials said:

A lot goes in calculating few parameters!!! I will start with manufacturer's numbers and move forward from there.

Just curious if anyone know, how do manufacturers come up with numbers? Do they just go till the tool blow up and take average or something?

Check out chip thinning. It's already been hit on here but not named exactly. With modern software, this theory is crucial to fully understand. 

Lots of stuff on the intard net about it.

 

Edit: While you are doing that, look up dry vs. wet machining and how coatings work as Ron mentioned.

Edited October 19, 2023 by cruzila

[Jake L]

19 hours ago, Jobnt said:

Axial engagement will vary depending on radial engagement. Try different combinations to find what works best.

You can run full depth with > 75% radial engagement but your feed will be very slow.

Or you can run full depth with < 10% radial engagement and extreme feed rates.

Or you can run at < 5% axial depth with full radial engagement and feed stupid-fast but I've never gotten the MRR to be more efficient using the last method. Machines usually can't accel fast enough to hit those kinds of feed rates before it has to slow down for the next corner.

Agree with all of this. Will add that some end mill geometries are made specifically for a single one of these approaches.

Example, you won't have much success slotting with a 9 flute endmill in steel, but a light step over and full axial engagement with the same endmill will outperform a standard 4 flute endmill. 

[Metals and materials]

High Efficiency Milling, correct?

I have to program a part to remove all the materials except 4 fins in the center. I will try these. I will go full axial depth possible (100% flute length) with the lightest radial engagement about 5% and I will keep my feeds and spindle speed high (high SFM as well). The material is Titanium and tool is carbide TiAlN coated.  Hopefully, it will not scrap the part or break the endmill. 

[crazy^millman]

6 minutes ago, Metals and materials said:

High Efficiency Milling, correct?

I have to program a part to remove all the materials except 4 fins in the center. I will try these. I will go full axial depth possible (100% flute length) with the lightest radial engagement about 5% and I will keep my feeds and spindle speed high (high SFM as well). The material is Titanium and tool is carbide TiAlN coated.  Hopefully, it will not scrap the part or break the endmill. 

I have seen up to 400 sfm being run in TI and getting 120 minutes of tool life. Premium tools with the correct coating in a HD shrink on a Makino.

[Metals and materials]

13 minutes ago, crazy^millman said:

400 sfm

Ohh wooow!!!!

Let me ask you this then, I am using,                                  BTW I am using DMU monoblock 5 axis machine

1)YG-1: BEST VALUE IN THE WORLD OF CUTTING TOOLS (yg1usa.com)   to remove some material from the center. After reading all the suggestions, I am thinking to go 75% in stepdown and 5% in stepover/minimum toolpath radius with SFM of 75 ( which is a quite quite low compared to 400) and feed of 10/spindle of 1146. 

Now, I am thinking keep cut parameters the same, increasing the SFM to like 150 or something

[#Rekd™]

Another issue to be aware of is correcting your feed rate for helixing inside holes close to the diameter of the tool. HSM Advisor has a button for this.

 

[crazy^millman]

27 minutes ago, Metals and materials said:

Ohh wooow!!!!

Let me ask you this then, I am using,                                  BTW I am using DMU monoblock 5 axis machine

1)YG-1: BEST VALUE IN THE WORLD OF CUTTING TOOLS (yg1usa.com)   to remove some material from the center. After reading all the suggestions, I am thinking to go 75% in stepdown and 5% in stepover/minimum toolpath radius with SFM of 75 ( which is a quite quite low compared to 400) and feed of 10/spindle of 1146. 

Now, I am thinking keep cut parameters the same, increasing the SFM to like 150 or something

4 Flute I would push it up to 30% step over maybe 50% step over. 11 Flutes I run 3% step over up to 6%. 7 Flute 5% up to 9% Step over, 5% step over on a 4 Flute is watching paint dry. 75 SFM is leaving so much profit on the table not even something I can laugh about. You need some real mentoring and need to bring in someone like myself or Aaron. After one week of either of us in your shop profits will go through the roof.

[Metals and materials]

11 minutes ago, #Rekd™ said:

Another issue to be aware of is correcting your feed rate for helixing inside holes close to the diameter of the tool. HSM Advisor has a button for this.

This is helpful!! Thank you for sharing. 

[Metals and materials]

10 minutes ago, crazy^millman said:

4 Flute I would push it up to 30% step over maybe 50% step over. 11 Flutes I run 3% step over up to 6%. 7 Flute 5% up to 9% Step over, 5% step over on a 4 Flute is watching paint dry. 75 SFM is leaving so much profit on the table not even something I can laugh about. You need some real mentoring and need to being in someone like myself or Aaron. After one week of either of us in your shop profits will go through the roof.

Because of hole material limitation, I cannot go past 20%. I found that speed and feeds/SFM from machining doctor lol. 

But, true, I do need some good mentoring. I went to couple classes for trial but none of them were good. All they tell is very basic stupid stuff and charge a lottt. So I just keep researching online and try to find something I can put into practice. 

[crazy^millman]

Check out the attached from the catalog, Getting into the hole? Drill it out and then use the tool the correct way. No need to helix into the part. Drill a starter hole with a drill or flat bottom drill and then bring this in an rip out the material.

[Metals and materials]

Curious question, do you mentor??

Like this. 

[crazy^millman]

I would drill it out then come back and finish it. I would do 2 fins and make a stabilizer block and then do the other fins. I might do all 4 fins and then make a stabilizer block and then finish the inside. I would still drill the inside and then finish with an endmill. Drill is meant to make a hold. An endmill will make the hole, but not made for it. Then you can push the endmill, but this is where Physics kick in to the process and those thin ribs make us slow down not to bend them. Where a stabilizer block to support them will be a hugh help without it then what I was thinking has to be adjusted. Where again a lot of things have to be considered when coming up with a manufacturing process. With the thin ribs I might waterfall them from top to bottom. I might have roughed the part +.05 on each wall. Then came back and water fall finished stepping down with a small flute length, but extended reduced shank. Letting the strength of the material help me as I work my way down.

Harvey Tool