View Full Version : Haas vs hurco vs fadal cutting 316 ss.

luis hernandez
02-14-2004, 09:04 PM
Has any body cut 316L stainles steel with .040" carbide end mill with a basic unit or tool room from Haas,hurco or fadal. the cut has to be about .040" deep x .040" width. How many passes this could be done and fast before tool breakage.. any experiencing using one of those machines with this metal. We want to buy the machine within two month but we want to know which one can do this job before spent that kind of money. I heard that rigity will dramatically affect this type of cut. Also I keep hearing very bad things about Haas nad fadal.... any suggestions..


02-15-2004, 01:28 AM
Have the Haas dealer demo that cut for you under actual cutting conditions. That is a tiny endmill, but you should not have any real problems cutting it. The factors affecting the cut is the tool more than anything, and if it has to do any tuns deceleration in corners is important - the Haas and Hurco should both do well. with a small endmill like this you need high spindle speeds - the higher the better.

Talk to your machine dealers for an actual demo - this is the smart move on your part - they should be more than happy to comply with your request if it means selling a new machine.

02-16-2004, 12:04 PM
No experience doing it but, you'll need the Haas Mini-Mill as opposed to the their Tool Room TM1 mill so you get higher spindle speed. 7500 on the mini I believe as opposed to 4500 on the TM1. I can't believe bed and spindle rigidty is a big issue here as you'd flex and snap the tool long before you moved the bed. And to keep from snapping the tool, you need a fast spindle speed, small cuts, fast table travel/look ahead to cut machine time. Also ask sales engineer if there is a better way to machine your part...you might be suprised what they come up with. Big price diff between Haas/Fadal/Hurco, what do you want overall?

C. Tate
02-16-2004, 12:45 PM
Rough estimate you will need 14325 rpm to make 150 sfm which is reasonable starting place for 316. Feed rates on these machines are not an issue you will probably need to feed about 20 ipm at that RPM (.0005 ipt with 3 flute mill). I would suggest a high quality speed increaser. I can say that my FADALs are quality machines I own three.

luis hernandez
02-16-2004, 12:52 PM
I will be milling it from an .125" rod or bigger for rigity and using a collet monted on a rotary table. My calculation give me about 10000rpm btu I am wondering if the mill will last and how fast and can feed to produce more in less time. I think using a slotting saws will be better but I would have to use an angle head for this tyoe of cut. I am planing to go more than $35000 for the machine and rotary table..

C. Tate
02-16-2004, 02:02 PM
Slotting saw and rotary table with spindle parallel to table you will not need right angle attachment. Have you thought about a cobalt woodruff key cutter ground to proper size. This will be stouter than carbide and the number of teeth would allow you to feed quickly. For .5 dia tool at .o4 deep I would estimate 400 rpm and 15 ipm.

luis hernandez
02-16-2004, 02:14 PM
The parts haves different cut. they go all around the stock so it has to be place horizontally so I would need either a 2 axis rotary table or angle head. so the possible solution is to use an end mill. I am wondering if a mill/drill can be use for the initial cut using its small angle tip and then use the regular endmill and for final cut..

02-17-2004, 09:31 AM
The Fadals have a much better stronger spindle than the Haas...


luis hernandez
02-17-2004, 10:27 AM
I keep hearing that. fadal is a litle bit more rigit than haas. but I have sent several e-mails last week and nobody has responde yet. that tell me what kind of service they have so I took their machine out of my list. Haas sent me a full brochure, video, price list and they are ready to test a machine. I will have them cut make this cut and see if it can be done.

another thing that worry me is if the rod/stock is .125" how come it will withstand side mill with different cutters. I will have to use and bigger dia rod but then I will have to mill more material making the proccess slower. any suggestion guys..

02-18-2004, 04:28 AM

I don't think you will get much deflection with that small an endmill providing you do the cutting as close to the work holding collet as reasonably possible. Without a drawing of the part that is difficult to really say off the cuff - but have the machinery dealers actually cut he part and time it for yourself that is the only way you will know for sure my brother.

02-19-2004, 12:46 AM
I cut stainless in that scale with a Haas Mini-Mill nearly every day...electron microscope components. The Haas does an excellent job. It does everything that I want it to do and can hold +/-.0002" tolerances depending on my fixturing...very nice. In addition, the stainless likes to be cut at around 50ft/min with HSS. This works out to be around 5000rpm which falls under the spindle's top speed of 6000rpm. A four-flute endmill should really be the only choice...and actually, HSS works just fine. Figured at .0005in/rev, that figures to be a feed of 2.5in/min. If you take .005"-.010" cuts and flood with coolant, you should have no troubles. In addition, if you use a 1/32" e/mill, cutter comp can be used to hold tolerances that much tighter. That way, using several different tool offsets can keep the side as well as the end of the mill engaged with the part. You can try to take cuts with higher feeds or speed, but much over 50ft/min and you run into serious risk of work-hardening...even with coolant flooding.

luis hernandez
02-19-2004, 09:13 AM
you have mentioned HSS tools. What is the smallest endmill dia you can find in HSS?. Mine has to be around .040". has you cut with endmill this size?

02-19-2004, 10:42 PM
Luis I agree with Nathan on this one. I also use 1/32 HSS endmills almost daily to cut .040 by .040 grooves. I like the 1/32 better than the .040 because you can clean up the burr that the rough cut leaves. The speeds and feeds Nathan recommends are right on with what I would use. By the way the smallest endmill in HSS I have seen is .005, but the smallest I have personally used is .015 . I used it to cut a small groove manually on a bridgeport, needless to say it was no fun at all.

luis hernandez
02-19-2004, 11:03 PM
Well mochinist you have to tell me where to get those Hss end mill. I have about 15 catalog from supplier and none has hss endmill that size. Is there any website/limk you can provide? Are they expensive as carbide? why you guys do not use carbide instead?

luis hernandez
02-19-2004, 11:09 PM
My calculation give me 10ipm feed instead:

.0005" (feed per tooth) X 4 (flute) X 5000 (rpm) = 10ipm

please correct me if I am wrong. has you tried carbide?


02-20-2004, 03:10 AM
Go ahead and try it at 10 ipm and see what happens, just remember that is a small ass endmill. Here is a link to J and L's online catalog go about halfway down and you will see the endmills I was talking about , if you scroll back a few pages they have many more small endmills. I dont like carbide this small just because it is so brittle and I usually cut my grooves in copper, so it isnt neccesary for me to use it. Now quit thinking about it so much , buy a few different types of endmills and make some parts. That will be the best way to see what works for you.

[This message has been edited by mochinist (edited 02-20-2004).]

luis hernandez
02-20-2004, 09:25 AM
I think they are new on the catalog.. but you righ, small as .006". what kind of holder you use? a collect maybe? where do you buy your holders or collect for this tiny endmill?

thanks you for the advice..

02-20-2004, 11:24 AM
Luis those endmills have been in there for years, these machining catalogs just have so much stuff in them , that it is easy to miss something. As far as where we got the collets, I dont know. The style of collets we have for the Haas are ER-16, and the 1/32 collet will collapse quite a bit smaller. When I used the .015 endmill in the bridgeport I had to use a drill chuck(bad I know) to hold it because I had no other way. J and L has a tech line, and they are pretty helpful when it comes to stuff like this. good luck

luis hernandez
02-20-2004, 11:36 AM
I think your right. maybe I was always looking for carbide endmill instead. I always thought that stainless steel can be cut just by carbide when slot are these sizes but I was wrong..

[This message has been edited by luis hernandez (edited 02-20-2004).]

luis hernandez
04-02-2004, 04:22 PM
I am having a hard time finding a 4 flute 1/32". what pages you said it was. by thay I rum carbide and went .010" deep per pass and 2 ipm (8000rpm spindle) and works fine but If i go 3 ipm or .020" deep it breaks. I am wondering if I can get more with a HSS end mill..