Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

HST thoughts on 6AL-4v


crazy^millman
 Share

Recommended Posts

I am helping a customer with parts like this. Has 40 taper machines and thinking 20% step over with a 125% depth of cut is going to be too much for their machines. They are Mori-Seiki machines, but still it is 40 taper so I am leaning towards the 5% step over which means I can go upwards of 700 sfm and up to .004 per tooth. Using a 5 flute endmill I would be at 3560 rpm and 57 imp taking a 1" x 6" x 4" section of Material in about 14 minutes. If I get aggressive and go up in the my step over to 20% at my 125% step down I need to slow down to .0035 per tooth and 450 sfm. That is 2292 rpms and 32 ipm and would cut the same area in 7 minutes. The HSM Adviser is pointing to better tool life using the more aggressive step over and I would agree with that, but on these 40 taper machines I am just worried they will hold up for the next 4 years pushing them to hard. It is a 4 year contract for my customer so trying to weigh the balance of time and wear and tear on his old equipment. My customer wanted me to program everything with cobalt and 3 imp and think I have lost my every loving mind going in this direction. Has his cobalt endmills on stand by when the Carbide Endmills fail. :thumbdown: Needs to be able to produce the parts in a timely fashion and I am very confident in the HST toolpaths, but going back and forth between my crazy push it to the limits and get it done mode to a more conservative get it done, but be easy on the machines. Anyone who has worked with me knows I go not problem burning up tools to get the job done. Customer will be happy just getting the parts made and if they took 20 hours a piece to machine he would be happy. Problem is I see now way to produce 80 parts a month if you old school it. Need to HST these parts and would be able to hit his desired 80 parts a month capacity. Take an average amount of hours a month on a 30 day month and get to 720 hours and divide it by 80 part you have 9 hours per part to machine them. Thinking one spindle is going to do all the work is where is wants to be. I am thinking one HMC to do a majority of the work and 3 VMC's to od other operations be would be able to his his mark if we HST these parts. Going to Cobalt 3 ipm way is not going to make it happen.

 

Question do I push 40 taper 10 and 15 year old machines with 20% step over or do I take it easy and go to 5% step over?

 

Cobalt is not an option for me and I know some old school folks on here will be right here with this part telling me I am crazy, but seen these toolpaths in action and one customer I talked to this week on a part they use to do before HST toolpaths was taking 5 hours to rough after HST toolpaths were getting them roughed in 2 hours. Not 6AL-4v, but the principle is still the same.

 

I am open to other suggestion or comments about this.

Link to comment
Share on other sites

I have been machining 6-4 Ti for the last 5 years on 40 tapper machines with no ill side effects. I run at 300SFM with 15-20 % step over and up to 100 % depth of cut. I use SHUNK hydraulic tool holders when doing heavy milling. My end mill of choice is IMCO (yes hard to get sometimes but worth it for the $$ paid). I have not had any issues on any of the 3 machines we have 1 - 4020 FADAL, 1 - 6030 FADAL, and a VF3 HAAS. I have found that the type of coolant and the mixture percent also plays a large part in tool life. I run at 7-9 percent and using HANGSTERFERS 500CF. I understand HAGSTERFERS has newer out there but my coolant needs to be BOEING certified and approved not just compliant.

Link to comment
Share on other sites

I have a customer with a Haas vm3 cat 40 with a trunion. I usually take the 3-5% stepover approach due to rigidity issues from the set up. I run the Kennametal Harvi 3's 1/2 bull w/.03 -.120 radius six flute. 450 sfm 144 ipm 1.25" doc. I get about 4-5 hours in cut for tool life and the endmill costs about $65. Just food for thought.

Link to comment
Share on other sites

Depends on the machines, Ron, but I have always favored big stepovers/DOC on older machines... especially if they can handle it... in fact, some of the older machines with big, bulky cast iron heads do much better than late model CNC's on bigger stepovers,DOC.

 

JM2C

Link to comment
Share on other sites

Sorry thought I put 3/4 endmill in there. I have to got 3.5" deep reason I went with 3/4 endmill for 2nd and 3rd operations. Might come down to a 1/2 endmill on the prep op, only 1" deep, but going 3.5" deep with a 1/2 endmill on a part that will have .1 walls not something I was looking forward to trying. Part is meant for a 5 axis, but doing what I can on a 4th axis HMC with 1 deg indexing. Will be on a Vice Tower again not my idea, but trying to take what I am told I have to use and use it to the best of my ability. I did make up some dovetail jaws to hold the part and prepping it on the VMC. Slots in the part are 1.1" wide x 3.5" deep and I have seen better results with the HST Toolpaths verse High Feed endmills time wise. I have to finish up my design on a 4th operation where I am swinging the parts on a 47" arc to drill the holes that should be done on a 5th axis. Wit hthe 1 dge indexing there was now way to do them in one fixture even if cheated the angles to drill them.

 

Thanks for the feedback and trying to make it where we know it can run lights out so thinking the 5% step over might take a little longer, but should run unattended the best. Once we get into production on the 80 pcs a month then we can see about increasing the step over and see how they handle it and what effect has on the tool life. I will keep everyone posted since this will be my 1st full production job in a long time that will run for years on Ti.

  • Like 1
Link to comment
Share on other sites

Jeremy, it is a really good program and you can decide if you want to push it to the HSM limits or play it safr with the tool. The deflection is great to see and then you can adjust your speeds and feeds from there and see what it says about tool life and such. It of course cannot take rigidty into account and other things, but the projects I have used it on have been right where it said it should be.

Link to comment
Share on other sites

I've got a customer running Aluminum Speeds and Feeds in Ti on a RoboDrill. It's the ONLY way to fly IMHO. You're not going to beat that machine up too badly living around 150 IPM.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...