Where to start dynamic feeds/speeds

[champshire]

Looking for some advice as I don't really know what to think of HSM Advisor's numbers. Looking at 4340 material that is 40 RC. 7 flute 3/4 solid carbide endmill ( https://www.garrtool.com/product-details/?EDP=64380 ). 1" doc, 2" stickout. .060 Radial (8%). Cat 50 Makino, great fixturing. Techniks mill Chuck. What Garr says and HSM says are totally different. What would you start with for feeds/speeds? Thinking .003/.004 a tooth and 400 sfm, but I am thinking this may be way conservative?

Disclaimer...I haven't really used HSM Advisor, the first real project is this one. Also, done very little dynamic milling as well. I would like some real world experience if possible please.

[CNCAppsJames]

The more rigid the setup, the higher quality the toolholder, the more you can get on the high side of the cutting parameters. Personally I'd go to the high side of the SFM and middle of the chipload range. Check the tool wear after the 1st cycle. If no wear is visible then increase by 25% of the remaining chipload. So if I'm at .003 and my max is .004, then the next cycle if no tool wear was visible then I'm going for .00325. If all is good then .0035, all is good then .00375, etc... also keeping an eye on spindle load.

JM2CFWIW 

[champshire]

Now that I'm at work, I can get actual numbers. If I type into Mastercam's dynamic tool path and click RCTF box, I get 2037 RPM and 107 IPM. When I use HSM Advisor, and click chip thinning, I get 2147 RPM and 160 IPM. If I then turn on the HSM Box, it goes to 3956 rpm, and 295 IPM. Should I not be using the HSM Box? This is all at .004 a tooth and 400 sfm. Feed may be a bit much at .004, but I was just trying to compare apples to apples.

[JakeL]

Using the Garr numbers (325-490 SFM / .0028-.0048 CPT) I'll use the middle numbers 407.5 SFM and .0038 CPT.

407.5 SFM ~ 2076 RPM

For the CPT you can use Garr's chip thinning formula [.5 x (dia/stepover)] / [sqrt((dia/stepover)-1)] x CPT = New CPT
Plugging in 3/4 dia, .06 step, .0038 CPT results in .007 CPT.

.007 CPT ~ 101.7 IPM

These numbers (and the numbers you got) look a little fast but about right. 165 IPM might work, but I think you'd be looking at a broken endmill. 295 IPM sounds dumb.

I've also only ever used HSM Advisor like once so I won't be much help with that

[Jeff]

Looking for some advice as I don't really know what to think of HSM Advisor's numbers. Looking at 4340 material that is 40 RC. 7 flute 3/4 solid carbide endmill ( https://www.garrtool.com/product-details/?EDP=64380 ). 1" doc, 2" stickout. .060 Radial (8%). Cat 50 Makino, great fixturing. Techniks mill Chuck. What Garr says and HSM says are totally different. What would you start with for feeds/speeds? Thinking .003/.004 a tooth and 400 sfm, but I am thinking this may be way conservative?

Disclaimer...I haven't really used HSM Advisor, the first real project is this one. Also, done very little dynamic milling as well. I would like some real world experience if possible please.

If it were me, I would run it at 530sfpm, .0075ipt and 5% stepover. And no more than 1.5" d.o.c.
This is from a Sandvik Dura Mill spreadsheet that I use.

[champshire]

So no one thinks 300 IPM is a good starting point? 

[Jeff]

So no one thinks 300 IPM is a good starting point? 

HSM advisor needs to be setup correctly. It takes some doing, but once you do you'll get numbers better in line with how it "should" be ran.

[neurosis]

So no one thinks 300 IPM is a good starting point? 

You could get away with that using the right step-over.

[SuperHoneyBadger]

Just a stupid Q....but have you had the machine feeding at that before?
If you're used to HS paths then all is well.
If you're not and you've not got the machine highspeed codes activated or the machine parameters aren't configured, at those rates you could be in for a very bumpy ride as the machine bangs itself to pieces on direction changes.

"Round all my corners, Senpai, HARDER"

[champshire]

So I understand that the lighter radial doc the faster I can go. But HSM Advisor and Garr are worlds apart. I'm going to start at about 107 tomorrow and see how it shakes out.

This is a Makino a81x horizontal vintage 2015ish I would guess. Pretty nice machine. We do some high feed milling in it now. I am going to get schooled in their Super Gi on this project too. Lots to learn and that's fine with me.

Obviously this is a roughing operation and I am leaving .030 everywhere so I imagine I will be ok. I guess I will know in the morning.

I would like to know what I did wrong in HSM Advisor. If I uncheck the HSM box it comes up with feed/speeds that are more believable.

I appreciate the feed back from you all. There isn't much of an application for Dynamic milling when making crankshafts, but I think it has a place here on these connecting rods. Should be fun!

[HSMAdvisor]

Hello,

I was lurking around seeing what people say about HSMAdvisor and decided to register fore someone wrechs something because of misunderstanding.

It looks like the issue the OP is having is applying the Chip Thinning twice.

See, you enable Chip Thinning on HSMAdvisor and it suggests you the final feed rate and chip load.

But then you go to Dynamic Toolpath, enter HSMAdvisor' suggestions and enable CRFM which ALSO applies chip thinning to the final speed and feed.

You should be enabling Chip Thinning compensation only in ONE place, not both.

[neurosis]

I was lurking around seeing what people say about HSMAdvisor and decided to register fore someone wrechs something because of misunderstanding.

I don't think that you have to worry about that. 

Thanks for coming in and giving an explanation. 

Are you open to questions?

[HSMAdvisor]

I don't think that you have to worry about that. 

Thanks for coming in and giving an explanation. 

Are you open to questions?

Yes, of course I am open to questions.
If you have any regarding HSMAdvisor please ask via email or my support forums.

[champshire]

Update...

Worked on this project Friday and Saturday morning. We are taking Rods out of an older dual spindle Chiron VMC that is used up and putting them into a 10 year old Makino a81nx horizontal. Cycle time in the Chiron was 10:45 for a rod. I am strictly roughing it in at this point.

Using dynamic milling and a different tool with more flutes I reprogrammed it. It did not go as smoothly as I had hoped. The Makino did not like what I was trying to to do as it was jerking and slowing down even on straight away cuts. I changed settings in Mastercam (Arc tolerance and smoothing) and after several iterations I got it to run right.

I watched some videos off Makinos website on how to reduce cycle time Friday night as homework. I learned a lot about their special M codes they use. I put them in place on Saturday. They did in fact reduce cycle time. I was able to take close to 3 mins off what I had for 4 rods at the end of the day on Friday.

Cycle time is at 22:18 for 4 rods which works out to be about 5:35 a pc. I have some more playing to do tomorrow and I may reprogram two of the tools to start machining at the end of the rod closest to the tool changer. I also built an If statement into my programs as the machine was going to the tool changer door after every rod.

The dynamic milling is a success so far. I started at 2037 rpm and 107 ipm. I have not tried to turn it up yet, I am waiting on some non sealed collets for my mill chuck to come in so that I can blow thru air.

The special M codes and if statement I wrote will get applied to the other operations we use those mills for. I think I can save a bunch of time in those operations as well just by getting rid of non needed retracts and trips to the tool changer.

I'm sure this is all old hat to you guys, but it's been a fun project so far. I'm learning new things and thinking about every second of cycle time that I normally don't worry about.

I will be looking at the help section of HSM Advisor so that I can learn to utilize that better as well. I appreciate him taking the time out to chime in here and let me know what I did wrong.

[CNCAppsJames]

Generally speaking machines WILL perform better when using the High Speed modes either their builders or control manufacturers integrated into the machine. 

The myths persist about them. 

Know this, no matter what some Grey-haired codger that's been at the company since the late 70's. He's passing along outdated information that has been dead wrong for the better part of 3 decades. And unfortunately, SO many AE's in the industry aren't much better.