Invar.: Ever machined it?
Close
Login to Your Account
Results 1 to 17 of 17
  1. #1
    Join Date
    Apr 2004
    Location
    Mesa, AZ
    Posts
    162
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Post

    The boss put out a job today that is a part made out of Invar. It is gonna be a 6"X6"X.250" plate with a 1" square threw pocket and a 2" square pocket .150 deep on top of the threw pocket. The corners have a .079 radius called out on them and the pockets have a plus .0015" and minus .0000" tolerance. I have some nice 4 flute carbide stub endmills already and I am planning on doing this in the HAAS cnc mill. I was told that this material machines similar to 316 but it was the end of the day and I didn't have time to look it up. So is this true, my cad package doesnt have invar as a material I can select so should I go with the 316 stainless. Does it work harden like 316, and what kind of speeds do you recommend. I will definitely rough it out with something bigger but any help is appreciated asI had never heard of the material till today.

    Thanks

  2. #2
    Join Date
    Sep 2004
    Location
    Posts
    47
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

  3. #3
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,034
    Post Thanks / Like
    Likes (Given)
    13823
    Likes (Received)
    10686

    Post

    Don't even begin to think that something with a 30+ percent nickel content will machine anything like 316. Its essentially inconel. I just did a couple of big jobs out of A286, (same family), and I did a lot of research and talked to a bunch of sales and tech people, and also did a whole lot of experimenting. I would suggest ceramics if you have to do any big roughing 1000-7000sfm, it took our roughing time from 24minutes with carbide roughers to 17 seconds, its really cool, looks like your machine is going to catch on fire, sparks everywhere, I made a crappy video with a digital camera, about 4 megs, e-mail me if you would like to see it.

    On the other operations, treat it like aluminum. You really need to get underneath it and lift the chip out. We tried a couple of inserted cutters, but when the inserts failed, you had little to no warning and usually lost the holder, so we stuck with the carbide. We used half and quarter inch carbide roughers. Now here is the wierd thing, 70sfm on a particular path gave about 180 minutes of tool life, change to 100sfm and tool life jumped to almost 300 minutes (same chip load and path, its a mazak, so you set surface feet and chip load), jumped up to 130sfm and got 360 minutes of tool life, just over that and tool life was best measured in weather or not I could get a cup of coffee before it broke.

    Another strange thing, at first we were buying TiAlN coated endmills and then somehow ended up with a mix of coated and uncoated, on average, the uncoated had about a 30% better tool life than the coated.

    On the mazak with the 1/2 carbide roughers I was running up to .004 chip load per tooth, with a small step over of .135-.170. Running into a sharp corner as it appears your going to be doing I was really backing off on the chip load to a little over .001 per tooth.

    On these parts we ran the first OP on A mazak FJV25(where 90% of the roughing took place), bridge type machine, where we could really pile the coals on and then ran Ops 2-6 on a Fadal,(these ops were mainly picking away with small drills and endmills) where we had to back off on the depth of cut and chip load on the bigger cuts due to the machine trying to shake itself apart.

    Good luck, I hope this helped out a bit, I also hope you don't have to do tons of these, this high nickel crap gets real old real fast. On the work hardening thing, I didn't have a problem with it, even after running dull ceramics on it. Now for a shameless plug for a good supplier, we were getting our endmills from Cutting Edge in colorado. Nobody could touch their prices for the quality, 1/2" roughers for well under $40. 1/4 roughers for under $25. Get on a blanket order and it drops considerably from there.

  4. Likes BSCustoms liked this post
  5. #4
    Join Date
    Mar 2005
    Location
    Canberra, Australia
    Posts
    592
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Post

    Bobw,
    Invar is used because at room temperature is has almost zero coefficient of expansion, but that changes a little if you work it, and it may need heat treating to get the zero coefficient back - so I've read. Any requirement from your customer about this? Sounds like you were being less than gentle with it!

    Mike

  6. #5
    Join Date
    Sep 2002
    Location
    Lawrenceville GA USA
    Posts
    6,211
    Post Thanks / Like
    Likes (Given)
    759
    Likes (Received)
    1336

    Post

    I have had no trouble machining this material with carbide endmills. You do need to maintain a constant cut with it like you would with ss but with a good sharp carbide tool it machined well. The trouble I had was with drilling it, the drills wouldnt last more than a few holes. I finaly got the job done but I never was happy with my drilling. I would have liked to try a different drill or perhaps a carbide drill but there wasnt time to order one and I havent needed to work with invar again. I didnt even try to machine tap the holes, I just used Moly-Dee and hand taped the few holes I had to do.

    Good luck on your project, I woulndt let it scare you that bad but I would suggest a qood quality drill with a contant feed for a starter hole.

    Invar does need to be stress relieved post machining in order to restore its thermal stability properties. Although with the minimal amount of machining you are suggesting I dont think it will be neccessary. The material I had was A36 Invar, it was very rough surface and way oversize, .280 on a 1/4 plate. I cut it down with a carbide fly mill on a bridport but I would have had good success with a shell mill too.

    Charles

  7. Likes BGL liked this post
  8. #6
    Join Date
    May 2004
    Location
    Nebraska
    Posts
    413
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    14

    Post

    It machines better than A286 or 718 Inconel, if you have rigidity and horse power try a Green Leaf WG300 round with a T1 edge prep.

  9. #7
    Join Date
    Jul 2002
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    4,413
    Post Thanks / Like
    Likes (Given)
    731
    Likes (Received)
    623

    Post

    Bobw,
    Invar is used because at room temperature is has almost zero coefficient of expansion,
    That is exactly why we use it in our laser systems. These laser systems can be real sensitive, alignment wise, with temperature variations. We use a lot of optical elements made of fused silica (a glass). Invar is oftem called for as a mount material as its exp coefficient closely matches fused silica.

    Mark

    http://www.fibertek.com/

  10. Likes BGL liked this post
  11. #8
    Join Date
    Apr 2004
    Location
    Mesa, AZ
    Posts
    162
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Post

    Thanks for the help, I ended up doing it on the bridgeport, I rougher it with a .25 carbide endmill and then finished it with a .125 endmill. It wasn't the easiest machining stuff but it wasn't bad either, the hardest part was the initial plunge cut to remove the material in the center.

    The zero expansion is supposedly why the customer is using this, I also machined some small 304 stainless keys that fit in the pockets edges, he is going to use these in a high heat enviroment to hold a pc chip in for testing. The keys are supposed to expand and lock in the chip at the high heat. Thats all I know or could say about this without risking violating my confidelity agreement.

  12. Likes BGL liked this post
  13. #9
    Join Date
    Jul 2017
    Country
    SLOVAKIA
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Is Invar machinable with diamond tool? What parameters should we use?

    Thanks,
    Miroslav

  14. #10
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    California
    Posts
    588
    Post Thanks / Like
    Likes (Given)
    133
    Likes (Received)
    219

    Default

    mochinist,
    You are working with a material that has military implementations. The fact that you never seen it before, and/or have no idea how to approach it's machining is troubling to me.
    otrlt

  15. #11
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    7,494
    Post Thanks / Like
    Likes (Given)
    1763
    Likes (Received)
    5215

    Default

    Quote Originally Posted by otrlt View Post
    mochinist,
    You are working with a material that has military implementations. The fact that you never seen it before, and/or have no idea how to approach it's machining is troubling to me.
    otrlt
    Otrit, that you didn't notice this is a resurrection of a 2005 question bothers me!

  16. #12
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    7,494
    Post Thanks / Like
    Likes (Given)
    1763
    Likes (Received)
    5215

    Default

    Quote Originally Posted by ememtal View Post
    Is Invar machinable with diamond tool? What parameters should we use?

    Thanks,
    Miroslav
    Invar is a nickle/iron alloy, carbon level for Invar 36 is around .12%. My understanding is that diamond cutting tools are at risk of chemical degradation when exposed to carbon components in alloys at high temperature, but you may decide to do light finishing machining with it. I would not use diamond for rough machining, look to proper coated carbides instead.

    Is this for composite mold fabrication, or something else?

  17. Likes BSCustoms liked this post
  18. #13
    Join Date
    Aug 2006
    Location
    california
    Posts
    131
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    5

    Default

    From 2005.

    Quote Originally Posted by Bobw View Post
    Don't even begin to think that something with a 30+ percent nickel content will machine anything like 316. Its essentially inconel. I just did a couple of big jobs out of A286, (same family), and I did a lot of research and talked to a bunch of sales and tech people, and also did a whole lot of experimenting. I would suggest ceramics if you have to do any big roughing 1000-7000sfm, it took our roughing time from 24minutes with carbide roughers to 17 seconds, its really cool, looks like your machine is going to catch on fire, sparks everywhere, I made a crappy video with a digital camera, about 4 megs, e-mail me if you would like to see it.

    On the other operations, treat it like aluminum. You really need to get underneath it and lift the chip out. We tried a couple of inserted cutters, but when the inserts failed, you had little to no warning and usually lost the holder, so we stuck with the carbide. We used half and quarter inch carbide roughers. Now here is the wierd thing, 70sfm on a particular path gave about 180 minutes of tool life, change to 100sfm and tool life jumped to almost 300 minutes (same chip load and path, its a mazak, so you set surface feet and chip load), jumped up to 130sfm and got 360 minutes of tool life, just over that and tool life was best measured in weather or not I could get a cup of coffee before it broke.

    Another strange thing, at first we were buying TiAlN coated endmills and then somehow ended up with a mix of coated and uncoated, on average, the uncoated had about a 30% better tool life than the coated.

    On the mazak with the 1/2 carbide roughers I was running up to .004 chip load per tooth, with a small step over of .135-.170. Running into a sharp corner as it appears your going to be doing I was really backing off on the chip load to a little over .001 per tooth.

    On these parts we ran the first OP on A mazak FJV25(where 90% of the roughing took place), bridge type machine, where we could really pile the coals on and then ran Ops 2-6 on a Fadal,(these ops were mainly picking away with small drills and endmills) where we had to back off on the depth of cut and chip load on the bigger cuts due to the machine trying to shake itself apart.

    Good luck, I hope this helped out a bit, I also hope you don't have to do tons of these, this high nickel crap gets real old real fast. On the work hardening thing, I didn't have a problem with it, even after running dull ceramics on it. Now for a shameless plug for a good supplier, we were getting our endmills from Cutting Edge in colorado. Nobody could touch their prices for the quality, 1/2" roughers for well under $40. 1/4 roughers for under $25. Get on a blanket order and it drops considerably from there.

  19. #14
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    992
    Post Thanks / Like
    Likes (Given)
    1127
    Likes (Received)
    648

    Default

    Quote Originally Posted by claya View Post
    From 2005.
    Whats your point?

  20. #15
    Join Date
    Oct 2019
    Country
    CANADA
    State/Province
    Ontario
    Posts
    8
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    3

    Default

    I cut a bunch of INVAR at my previous shop, we just used coated carbide that was made for cutting aluminum. One thing you should note about that material is that is likes to spring a lot, so what we did for the spring is rough one side, flip rough, release part re-clamp with shim to not bend or warp part, semi, finish, then flip and do the same clamp and semi cut and finish cut process.

  21. #16
    Join Date
    May 2009
    Location
    Canandaigua, NY, USA
    Posts
    2,855
    Post Thanks / Like
    Likes (Given)
    138
    Likes (Received)
    1258

    Default

    I think there's a free cut version and regular. Try to get the free cut if the customer's OK with it.

  22. #17
    Join Date
    Dec 2013
    Location
    Spennymoor, England
    Posts
    55
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    19

    Default

    Invar was used on Moore Jig Borers for the quill housing casting as it has a negligible expansion rate when it warms up. Helps to maintain the accuracy of the machine


Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •