On topic - Kovar

Tips and or tricks needed for turning this "stuff". I am currentley running 120 sfm, .006 roughing / .002/.004 finishing, having a wee bit of trouble staying on top of the dimensions.

Anyone with some ideas?

TIA "D"

Reply to
reidmachine
Loading thread data ...

Snipped from a site. SFM may on the low side, according to these references. DOC is also pretty shallow. Haven't cut Kovar yet. Similar to Monel, I understand.

The espi-metals has some interesting info. Worth looking at.

ca

Coolant It is important to control heat build up, the major cause of warpage. A suggested coolant would be Cool Tool. Cool Tool contains fatty esters to reduce friction in the cutting zone and a refrigerant to remove the heat generated by friction between the cutting tool and work place.

Tooling T-15 Alloy, such as Vasco Supreme-manufactured by Vanadium Alloys Company. M-3 Type 2, such as Van Cut Type 2-manufactured by Vanadium Alloys Company. Congo manufactured by Braeburn. For machining with carbide tools, a K-6 manufactured by Kennemetal, Firthie HA manufactured by Firth Sterling, or #370 Carboloy could be used, or a K2S manufactured by Kennemetal, or Firthie T-04 manufactured by Firth Sterling would be satisfactory. One thing of prime importance is that all feathered or wire edges should be removed from the tools. They should be kept in excellent condition by repeated inspection.

Turning If steel cutting tools are used, try a feed of approximately .010" to .012" per revolution and a speed as high as 35/FPM could probably be attained. Some of the angles on the cutting tools would be as follows:

  • End cutting edge angle -Approximately 7° * Nose radius -Approximately .005" * Side cutting edge angle -Approximately 15° * Back rake -Approximately 8° * Side rake -Approximately 8°

When cutting off high speed tools are better than carbide tools, and a feed of approximately .001" per revolution should be used. The cutting tools should have a front clearance of about 7° and a fairly big tip--larger than 25° would be helpful.

formatting link
formatting link

Reply to
clay

Thanks Clay, I was thinking about sneaking up on 225, doc is going to stay the same, the biggest fit is coming from a .01 rad corner relief @ 1.239

+/-.001 dia, recessed in the face .02 deep, friggen tip keeps popping off, less feed!!

"D"

Reply to
reidmachine

snipped-for-privacy@msn.com wrote in news:b4318f7c-d2b2-452e-b139- snipped-for-privacy@z16g2000prn.googlegroups.com:

Sharp positive rake tooling works best. I would say that your SFM is in the ball park for coated carbide, if anything you might be running a little fast. Uncoated I would use a micrograin carbide at around 90 SFM for finishing a little slower yet for roughing. I've used Kennametal KC735 grade and it worked OK, not great.

If all else fails switch to HSS. I used to use a chill cast HSSCO tool bit from a company called "Blackalloy" for Kovar. They also made HSS inserts like TPG's in HSSCO. Run around 35 SFM with the HSS.

Nowadays I would try a Sandvik CCMT 32.51 MF insert in GC-1105 grade. I haven't had the chance to try it in Kovar but it was by far the best thing I've seen in MP35N and 718 Inconel. So I'm guessing it should work well in Kovar. Very sharp despite the coating and positive rake to boot. Otherwise try a Kyocera Ceratip insert. IIRC, PR930 would be the best grade but I would check that before ordering them.

Kovar is a controlled expansion alloy usually used for glass sealed hermetic connectors, etc. It's a bitch. It has a lot of iron in it. So it wears the tools down in a hurry and it doesn't like speed or high feed rates. I've always cut it with a straight cutting oil. The thicker the better with plenty of EP additives.

If you have to bore it, I've found two flute carbide end mills work well and offer good economy vs solid carbide boring bars.

Reply to
D Murphy

And there you have it. some say faster, people that have run it, say slower. but from all places, it seems sharp tools, lots of rake, expect to replace them often.... and cutting oil, thicker chips...

ca

Reply to
clay

My ISCAR rep used to say not to take a cut less than the tip radius. If you think about it, if you are taking a cut at half the tip radius the cutting edge is engaging at a 45 degree angle which will push more.

Will

Reply to
Will

Ok, here's where I ended up OD turn 225 sfm, .008 ipr for rough, .004 for finish ID 300 sfm, .004 finish after plunging hss/co endmill at 40 sfm and .

002 ipr, all tools holding up well drilling with co at 40 sfm, .004 ipr

"D"

Reply to
reidmachine

thanks man, going down in the future book.

ca

Reply to
clay

snipped-for-privacy@msn.com wrote in news:89ba29f7-6e1d-4277-a0a9-b6993a1e8001 @u36g2000prf.googlegroups.com:

That's on the hot side. What brand/grade carbide?

Reply to
D Murphy

That's what I thought, but it is running that way. Ingersoll WNMG- 432 grade TT5030 Same grade on rough bore tool, and uncoated c-6 for finish bore. uncoated needs dressing about evey 30 pcs, havent changed coated tools yet, run 150 pcs so far.

"I can argue with opinion, but I can't argue with results"

"D"

Reply to
reidmachine

snipped-for-privacy@msn.com wrote in news:3fd2c444-93e0-4709-859d-4d03805deb02 @w1g2000prd.googlegroups.com:

I think that TT5030 grade is similar to the Sandvik grade I was talking about. Ingersoll has some really nice stuff nowadays.

The results you're getting with the uncoated tool are more along the lines with what I would expect. It's been a while since I've machined any Kovar. I guess it follows that these newer grades for superalloys would work wonders with Kovar too.

Reply to
D Murphy

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.