Help with DOC/feed&speed/best order of operations?

Cerberus

Cerberus

Registered
Registered
Joined
Jan 24, 2018
Messages
11
Hi, so I have these parts I'm to make and have to make many of them. I'm starting with 6061 2.5 inch bar stock. The ends are 5.813 long and need to be turned down to .750. I want to take around .100 DOC per pass. What are the best feed and speed rates you guys recommend? I've been kind of "winging it". I've been doing about 290 Rpm and as for feed rate well... So my Fortune Lathe has a feed chart that says .001/rev but the numbers in the table are represented as whole numbers like 3.68, 1.83, 7.57 this doesn't make much sense to me because I'd expect to see .002, .005, .010 etc. etc. But I assume it means 3.68 is .00368/rev? Correct? IDK... I was using the whole numbers in my algebra as IPM not IPR. But the machine clearly says .001/Rev. I was getting lucky just going on sound and feel but kept either building up aluminum after a while on the carbide and/or bulldozing aluminum over the cut path. I would get decent chip formation, thick hot 6's at times and decent looking finish but the results were inconsistent and the part got quite hot. I've basically been using 300sfm as a start point for my aluminum calculations which I've seen anywhere from 250-500sfm for aluminum depending where I look and I know these surface speeds are for HSS not carbide but my lathe only does 1500 Rpm and honestly don't like going over 700 rpm. I've been using a simple turning calculator found here http://www.custompartnet.com/calculator/turning-speed-and-feed I'm curious how depth of cut comes into these equations or doesn't it? It's a 15hp engine. Could someone shoot me a few pointers with all this information?
 
2 1/2 " round down to .75" X 5 13/16 long to a shoulder? Correct so far.

If so you are holding the end with a live center no? One of the unfortunate drawbacks of that material is chip formation or lack thereof which means that low DOC and feed rate will cause the chips to get out of hand. If the machine and setup can handle it and using tooling designed for this material with flood coolant there is no reason not to turn it at 700+ fpm, .100" doc at .012-.015 IPR feedrate for roughing.

FLOOD COOLANT WILL BE REQUIRED

Push everything until the chip behaves and you do not have to watch it the entire time.
 
Wreck™Wreck said:
2 1/2 " round down to .75" X 5 13/16 long to a shoulder? Correct so far.

If so you are holding the end with a live center no? One of the unfortunate drawbacks of that material is chip formation or lack thereof which means that low DOC and feed rate will cause the chips to get out of hand. If the machine and setup can handle it and using tooling designed for this material with flood coolant there is no reason not to turn it at 700+ fpm, .100" doc at .012-.015 IPR feedrate for roughing.

FLOOD COOLANT WILL BE REQUIRED

Push everything until the chip behaves and you do not have to watch it the entire time.
Click to expand...
Thanks for the reply. Yes live center was used in tail to support the cut, I was however cutting dry. It's a 20 something inch long part with .750 shafts 5 13/16 long at both ends with a 9 inch long 2.188 diameter body in the center. It needs to run true the entire length and still trying to figure the best process/order of operations to machine it. I center drilled both ends then turned everything down leaving .050 over on the .750 diameter and .080 on the 2.188 diameter. I hate using lathe dogs so I only want to turn it between centers for finishing passes. Is my logic flawed? This is being done on a manual lathe and flood coolant isn't an option...
 
Curious to know which insert you're using. The maker will give you the cutting conditions, which will be impacted by the grade and chip breaker you're using. They should give you speed, feed and roughing depth of cut. Based on the nose radius and how the insert likes to cut, you can determine the best finishing depth of cut by trial and error; typically, this will be 1/3 - 1/2 the nose radius. Finishing feed rate is usually 1/3 to 1/4 the nose radius in IPR. Most insert makers will also give you their recommended cutting fluid for the material the insert is suited for but they may or may not tell you if this is for flood coolant conditions (the norm for aluminum machining).

You mentioned it has to run true. To me, that is a tall order on a 20" part that is going to deflect. If you turn it between centers then the use of a follow rest is going to be problematic with that big diameter in the center. Is it possible to hold the part by the larger center diameter and turn down the ends? What kind of tolerances are you looking at? What is the part for?
 
This is the insert... 20180125_100347.jpg
Tolerance is +/-.005

1st part I ran was within spec, 2.188 diameter only had .002 wobble, and didn't turn between centers, got lucky I think but the part took longer than I'd like.
 
I don't use WNMG inserts (trigon) but they're popular. A positive rake insert. Yours is an obsolete one and hard to find info on but Corokey is Sandvik. This particular insert is intended for use on steel - carbon, stainless and cast - but not aluminum. It has a 0.031" nose radius on it so fairly large.

So, this is the wrong insert for aluminum and the cutting conditions given on the package apply to steels only. Do you have an aluminum cutting insert available? An uncoated AK or AL insert would be good.
 
Thank you for the advise, I should've guessed it wasn't for aluminum. These were found around at work and I admit I just threw it in and away I went. I'll look into getting the boss to order some carbides ment for aluminum. I shouldve looked them up before hand. Surprised they worked as well as they did to be honest. Uncoated work better on aluminum?
 
I prefer the AK inserts for aluminum; I have not used the AL geometry myself. These come in different shapes but the AK geometry has a very positive rake, is ground and polished, the chip breaker works well and the insert is very sharp. Most of these are uncoated (H10 grade) and work well in aluminum for both roughing and finishing. I don't know if they make then in a trigon shape (WNMG), though.
 
I run WNMG inserts set up for aluminum, I use Korloy HA H001 type and you can get almost a mirror finish with good cutting performance. The AK inserts are more positive and may be a bit more fragile if taking a deep DOC. The HA is also a positive cutting edge insert but a bit better supported, both are for fine to medium cutting in aluminum. HA can also be used for low carbon steel and stainless. I often use them for light finishing cuts with steel/alloys and cast iron. The H001 grade is a fine grain polished carbide, usually you do not use coated inserts in aluminum, but there are many variables so for Kennametal they use a KC-5410 coating (insert for aluminum is a WNGP080408K). I use the Korloy inserts for aluminum, you would probably be looking at the Korloy WNMG080408-HA H01 / WNMG432HA H01, a WNMG431 may be too fine a tip if you need to do a lot of metal removal.
https://www.suncoasttools.com/crm/ItemPage.aspx?ItemNumber=17WNMG432HAH01++++KR&VendorNumber=KORLOY
 
You must log in or register to reply here.
Back
Top