High speed roughing help...

[brandon b]

Attached is my a section of the part im working on.

material TI 6-4 AL V

machine is Fadal VMC 6030 3 axis 10,000 max rpm.

FEEDS CANT EXCEED 200 IPM

 

Tool is PCT 3/4 4flute cobalt wave cut

 

 

I have attached 2 toolpaths. the first one is how weve been doing it. the second is how I would like to do it.

do my parameters look "realistic" . The boss doesn't see how the cutters can hold up to running this fast in TI.

TTT.MCX-7

[brandon b]

Just remembered I put the wrong step down in the second tool path

[crazy^millman]

Brandon you can erase the file and reload the new file with the correct depth of cut. Were you thinking .75 step down? I would think along those lines and look at the same step over or maybe as much as 10%.I read this endmill and look what it can do.

 

http://www.1helical....ges/hxvrcat.pdf

 

Looking at your current method backplot shows 8 hrs 37min and doing with 10% RDOC and 100% ADOC you should be able to run between 160-220 SFM and .0037-.0045 feed per tooth on a 5 flute endmill. They consider anything under 15% RDOC light duty roughing and anything in the 25% to 35% Heavy Duty with a 5 flute and if going down to a 4 flute with that style of endmill 35% to 50% Heavy Duty Roughing. I would think a 50 taper would be needed for that aggressive of a step over in Ti. I went to the somewhat aggressive side with 200 SFM and .0045 per tooth feed rate with a 10% step over. I see a backplot time of 1hr 45mins. I would have no problem going though an endmill part for a run time reduction like that. Take a standard $100/hr shop rate and got 7 hours reduction using this method that is $1400 turn around on a $200-$300 endmill per part. Use the High Side cost of $300 an endmill on 20 parts you made a profit of $22K going in this direction. Yeah tell him you I will buy the tool for the 1st part and if it works for the next run of 20 parts he gives me the profit.

[brandon b]

Ok so I'm thinking ill start at 7% stepover and maybe 75-100%adoc. 160 sfm the conservative side and go from there.

 

So you are estimating ill be using a endmill per part?

 

So far the "slow way" I've snapped two cutters and have only Gone around the first part 5 times .

 

 

 

[brandon b]

http://www.pctcutters.com/pct_product_PM30_series.aspx?Series=CC&NoOfFlute=4&ProdType=CoatedSquare&HandCut=R&Reach=0

 

 

 

How do you think these cutters will work for HSM ? These are what I'm currently using

[brandon b]

I'm using the 3/4

[THEE THAINZ™]

Brandon,

Have you tried using an Imco brand endmill? This is primarily the endmill I use in Ti, and like you I am using them on an older 6030 FADAL. Their M525 can be ran at 200 SFM comfortably and handle the chip load that Crazy recommended with good tool life. I cannot not view your file because I do not currently have MC7 loaded but can you use a smaller diameter endmill? If so have you thought about trying high speed machining your part? I am currently doing a part with a 1/2" endmill .400 "DOC .040" WOC 270 SFM and typically get around 90 minutes usuage per endmill. And biggest thing I have learned running TI is more flutes more better.

Merry Christmas

thainz

[crazy^millman]

Brandon their delivery sucks look to what I put up and 5 flute. Yes one end mill per part plan on it. With Ti you either old school it with Cobalt or New School it with HST and preinum tools. I would do my time study on 160 SFM verses 200 SFM and see if the difference is worth running it hotter. I have a customer who just picked a million dollar contract of Ti work and we will be trying this tool. I used the same logic in my quote for his work. We can spend 20 hours a part doing the 4ipm or we can do them in 6 hours apart feed them at 90 imp and 200 SFM. Trade off was more tooling, but my customer understood he did not have to get 4 more machines to do the work just needed to spend more on the tooling.

 

HTH

[brandon b]

I just said the pct cutters cuz that's what he bought for this job. It's only 5 parts and we won't see this part again.

 

 

This all makes logical sense to me but the one in charge is old school and....... Well you know that game.

 

 

I'm going to keep trying to go hst

 

 

Thanks for your help!!

[brandon b]

Thainz yes I can use a smaller endmill . I will have to look into it. Thanks and merry Christmas

[MIL-TFP-41]

Cobalt would not be on my list for any HSM. Looking at your part tho, I would look into using a high feed cutter, like a mitsubishi AJX style. With the smaller step downs that these style of tools use you will be closer to final shape when it comes to finishing.

[Brewster]

I highly recommend Helical Carbide endmills. I just finished up a Titanium 6al-4v job where the machine was running 56ipm with a .125 bull endmill, .150 adoc and .007 stepover. I really feel it could have been ran faster.

[brandon b]

So does it sound cost effective for me to use 3/4. Or a smaller endmill ? On this part I attached in the first post.

[THEE THAINZ™]

Brandon,

It would come down to tooling cost versus spindle time. All I run is Ti from completed assembled parts to target machined. I have not ever used the endmills that Crazy mentioned earlier but I will giving them a try to see if I can plug and play at the same parameters I currently use. If they last longer or reduce machine time by enough I'll be switching. I suggested the smaller end mill because of the ease of getting more flutes at a cheaper cost. If I could view your file I would give a better answer what is the biggest corner rad you can have during the roughing process?

[mkd]

sometimes slower is faster. old school cobalt method will get IT done for five peices that you will never see again.

 

Ok so I'm thinking ill start at 7% stepover and maybe 75-100%adoc. 160 sfm the conservative side and go from there.

confused: are these speed proposed for cobalt cutters? if so, i don't see it working. Need to drop to 40 sfm with cutter buried.

[crazy^millman]

You know I missed the Cobalt part of that tool description sorry about that. I am talking CARBIDE TOOLS not Cobalt sorry about that.

[brandon b]

Ya you had me going crazy, crazy lol. I'm just running it slow with these cobalt pct curve cuts until next week when we are guna have our tooling guy come in and help is.

 

I really wanna go to a indexable cutter. But we really haven't messed with any. What are your thoughts on indexable vs a solid endmill for roughing a part like this

[crazy^millman]

High feed cutters work very well, but you do throw stress back into the part using tools like that. Using the carbide endmills taking all the stress and heat out in the chip seems to do wonders for Ti and other metals. You got the cutter you got and yes you stuck to the SFM they give you again sorry I was going by you had gotten Carbide seeing those speeds and feeds and ran with it.

 

HTH

[mkd]

...

I really wanna go to a indexable cutter. But we really haven't messed with any. What are your thoughts on indexable vs a solid endmill for roughing a part like this

my experience with indexables in Ti was short lived. most general purpose (i.e. steel) inserts have a radiused cutting edge. it is only in the .001's" range but pretty much ruins their ability in Ti. maybe someone has a recommendation out there in eMC land, but i sure don't. combine this with the usual flute pitch being larger on indexable bodies seem to leave some money on the table regarding feed rates achievable.

solid tooling seems to be the way to go, IMHO. With the right part geometry cobalt can still perform very very well in terms of CU./min.

 

on second thought i have used some high positive button inserts on a F-22 structural part many moons ago. we were doing large swept surfaces and it worked pretty darn good actually. insert just need to be razor-sharp, G.P. won't cut it.

Edited December 25, 2013 by mkd

[reidmachine]

Brandon,

FWIW, I run a 1/2" endmill, .70 - .90 deep at 550 sfm and .04 step over (8%) on a minimill in 4340, (4200 rpm @ 90.00 ipm) I have removed an average of 105 lbs. of stock before the tool needs changing out.

I would assume that a $50.00 solid carbide endmill, vs. a $180.00 solid carbide (3/4) endmill would be a no brainer for an old school guy, and the cost of 5 endmills would be a lot cheaper than many hours on the machine.

 

I cannot view the file as I am away from my M/C computer, so, I don't know what the part looks like, but, I do know that a "Dynamic" toolpath, with a 1/2 endmill might just save you a ton of time and the boss a heck of a lot of money, Crazy would know the S and F's for the Ti, as I do not run a lot of it, but I would bet his #'s would yield some good results.

 

Good Luck

[brandon b]

This all makes sense too me. Just gotta get out there a try it. Just need some carbide. Tool sales guy should be out Monday.

[K2csq7]

We used a 3/4" Supermill here for a demo.... Roughed 6-4 Ti at 400 SFM.... tool cut for 1 hr... dynamic core... 50taper horizontal finished at 500SFM IIRC.

[mkd]

so how is it working out?

[brandon b]

Tooling guy gave me a 2 inch high feed. 4 inserts. .05 doc 1." Step over 30ipm 400 rpm.

 

I'm having a hard time figuring out how to program this tool. The od is 2 inches but the inserts are " angled in"? So I can only use a .75 step over or else it leaves large scallops that get taken out by the micro lift back feeds . It's a new tool and I can't find any info on it.

[brandon b]

All I know is its a Kyocera. Hard trying to get ahold of tooling guy. Some theives cut our phone line over the weekend and broke in and stole a ton of aluminum. Titanium , stainless . Fixtures and parts