Capability of VN22L--How big a cut?

[Reeltor]

I’m watching the videos of K&T’s, and Cincinnati’s taking huge cuts in one pass. I know a 22L is not a monster mill like a K&T, but it does have a NMTB 50 spindle. How capable is (or should be) a Van Norman 22L in the horizontal mode? I have both A & B arbor supports and 1” & 1-1/4” arbors; I don’t have an outboard support.
Yesterday I wanted to take a .370 wide cut, total of .100 deep in A-36 hotrolled. Using a 1” arbor and “B” support, I tried a 4” HSS wheel with 16 teeth, checking some on-line calculators; I came up with vastly different recommendations. One said to use 86 rpm at 2.4 inch/minute feed, the other recommended 1,400 rpm with a feed of 270-ipm.
I tried 95 rpm and feeds of 1.6 & 2.3 ipm. I tried a number of different depths of cut, from .030 through .060, the mill made a lot of noise.
I then tried the same cut using a 1-1/4” arbor, “B” support with a 6”-24-tooth carbide wheel. At 95 rpm and 1.6-ipm I got a washboard finish, so I increased the spindle to 180 rpm. The finish improved, and mill noise was the same at both settings. In hindsight, I think I should have tried slowing the spindle down, 50-rpm is the slowest possible.

For the most part I’ve used the mill in vertical mode cutting aluminum and it’s done everything I’ve asked of it. I do have the mill sitting up on 4x4’s so I can get a pallet jack under it when needed; do I need to put the machine down on the concrete and see if it makes a difference?

I want to take advantage of its horizontal capability, what should I expect from it (1954 build date)?

Mike

 

[DMF_TomB]

hp

I’m watching the videos of K&T’s, and Cincinnati’s taking huge cuts in one pass. I know a 22L is not a monster mill like a K&T, but it does have a NMTB 50 spindle. How capable is (or should be) a Van Norman 22L in the horizontal mode? I have both A & B arbor supports and 1” & 1-1/4” arbors; I don’t have an outboard support.
Yesterday I wanted to take a .370 wide cut, total of .100 deep in A-36 hotrolled. Using a 1” arbor and “B” support, I tried a 4” HSS wheel with 16 teeth, checking some on-line calculators; I came up with vastly different recommendations. One said to use 86 rpm at 2.4 inch/minute feed, the other recommended 1,400 rpm with a feed of 270-ipm.
I tried 95 rpm and feeds of 1.6 & 2.3 ipm. I tried a number of different depths of cut, from .030 through .060, the mill made a lot of noise.
I then tried the same cut using a 1-1/4” arbor, “B” support with a 6”-24-tooth carbide wheel. At 95 rpm and 1.6-ipm I got a washboard finish, so I increased the spindle to 180 rpm. The finish improved, and mill noise was the same at both settings. In hindsight, I think I should have tried slowing the spindle down, 50-rpm is the slowest possible.

For the most part I’ve used the mill in vertical mode cutting aluminum and it’s done everything I’ve asked of it. I do have the mill sitting up on 4x4’s so I can get a pallet jack under it when needed; do I need to put the machine down on the concrete and see if it makes a difference?

I want to take advantage of its horizontal capability, what should I expect from it (1954 build date)?

Mike

.
1018 and A38 is around 0.8 cubic inches removed per minute per hp
.
what ever motor you have figure getting maybe 50% of the hp at the cutter. so for example
.
5hp motor
2.5 hp available at the cutter
2.5 x 0.8 = 2.0 cubic inches milled per minute
........ some machines or parts vibrate before the hp limit is reached. you quickly after some time learn what a machines limits are.
.
roughing cutters the wavy corncob types in general use less hp, 1.0 - 1.6 cubic inches removed per minute per hp is very common

 

[sfriedberg]

I'm slightly more optimistic than DMF TomB about available HP at the spindle, but he's spot on with material removed per HP per minute. The Van Norman should be capable of reaching that limiting factor when properly set up. You should avoid climb-cutting, for example, until you know the table travel is solid and that there's no significant backlash. (Dunno if the 22L has one, but some later VN models had backlash eliminator mechanisms.) Learn how your machine acts when you (don't) have the proper axes locked down. Learn the difference between a sharp cutter and a dull cutter on your machine. (It can be a huge difference!)

Using your 16-tooth 4" diameter, 3/8" wide (or at least that much in the cut) HSS cutter example, I'd set RPM to 95 or the closest available spindle setting to keep SFM at or under 100. I'd set feed to 3 IPM to give each tooth a 0.002" bite. (Reasonably close to the results of your 1st calculator.) A 3/8" width of cut would allow almost a 1" deep groove per HP at those settings. So in principle, you could sink that cutter to the arbor, although I'd strongly prefer a 1.25" arbor rather than a 1" for that operation.

Using your 24-tooth 6" diameter carbide example, I'd set RPM to about 190 as a starting point to put SFM at about 250. I'd set feed to 9 IPM to give each tooth a 0.002" bite. Assuming a 3/8" width of cut, it would be a substantial load (if DMF TomB is correct, nearly a 100% motor load) to cut 1" deep at those settings. But 0.1" would be a walk in the park on a summer afternoon.

Both of those settings would be starting places. You don't want to try to take too small a bite per tooth, so there's a certain minimum feed rate for any combination of RPM and tooth count. You don't want to spin too quickly, so there's a maximum RPM for a given combination of work and cutter materials and cutter diameter. (Desirable SFM can be found in tables in many, many places.) You don't want to overload your motor, so there's a certain maximum material removed per HP per minute. You also don't want to overload your machine, but the VN (if in good condition) should stand up to anything its original 3HP or 5HP motor can cut.

Let's revisit "taking too small a bite per tooth". At 95RPM and 1.6 IPM feed, your 24-tooth 6" cutter was trying to bite only 0.0007" per tooth. That's definitely too small a bite. The cutter was probably rubbing (and dulling itself) and mangling rather than taking clean chips. When you increased spindle speed to 180RPM, keeping 1.6 IPM feed, you nearly halved the bite per tooth and I'm surprised you got any better results. (You also moved your carbide tooth cutter into a more productive range of SFM, which might have helped.) I'd say 0.002 to 0.003" per tooth is desirable in general, but you could go 0.001" to 0.004" per tooth if you had sharp cutters and a solid machine. So at 95RPM, feed your 24-tooth 6" cutter at 4.5 to 6.75 IPM. At 180RPM, feed
that cutter at 8.5 to 13 IPM. But at those higher feed rates, you will have to watch the combined width and depth of cut to avoid overloading the spindle. Still, 3/8" wide by 1/10" deep at 13 IPM is less than 0.5 cubic inch per minute, so piece of cake!

 

[Cal Haines]

I'm not sure about Mike's machine, but the one catalog that I have shows VN 22s having a 2 HP spindle drive motor. I don't believe that the table feed has an anti-backlash mechanism; at least there's no mention of one in the catalog or manual and the exploded views of the saddle and table don't show anything that looks like an anti-backlash mechanism, so climb milling should probably be avoided.

One problem that often comes up on machines that have been worked on by amateurs is gibs that are too loose. It's a common mistake to tighten them up until the axes feel nice and smooth, but that may leave them too loose; you should feel some drag when cranking by hand. Put an indicator in the spindle, with the tip touching the vise and try pushing and pulling on the knee, saddle and table, in turn (change the indicator position each time so that it's at right angles to the axis you're checking). If you can move the indicator just by pushing/pulling on an axis, the corresponding gib is too loose.

Cal

 

[sfriedberg]

I should add that a number of tool vendor tables give per-tooth milling feeds double or even triple my suggested 0.001-0.004" range, and the low end of the carbide on steel cutting speed range is usually listed as higher than my suggested 250 SFM. (SFM depends heavily on both material and its hardness.) Those higher numbers may be appropriate for production, after testing, but I would not use them as the starting point on one-off jobs.

 

[Reeltor]

I'd like to thank TomB, Sfriedberg & Cal for their responses. I will need to do some more experimenting in the horizontal mode to get a better feel for the machine.
I had to get a ladder to get a better view of the motor nameplate and was able to confirm that it is 3hp. I don't have a backlash eliminator; as far as I know the backlash eliminator was only available on universal table mills.
When I first got the mill I tried climb milling ONCE ; and that was one time too many! I adjusted the gibs after my climb milling fiasco and have them a little on the tight side; I'll have to put an indicator on and test for movement like Cal suggests.
I'll have to send a couple of cutters out to get sharpened so that I will be able to learn the difference between sharp and dull.
Thanks for all the help, its nice to know the machine should be capable, and the issue is most likely operator error.

From the comments, I think I was going in the wrong direction, taking too light a cut when I should have been more aggressive. I just took a .100 cut after readjusting the speeds & feed without issue.

Am I correct that taking too light a cut and the cutter to rubbing caused the rumbling noise?

Mike

 

[sfriedberg]

Am I correct that taking too light a cut and the cutter to rubbing caused the rumbling noise?

It certainly could, but other things are possible, too.

 

[kpotter]

I run my horizontal mill alot and have found that going slow and taking big cuts is much more productive than trying to run fast.

 

[johnoder]

You need to let each tooth do as much work as possible. Here is the opposite of rubbing the work piece and cutter to death. Steel, 6" wide, 1/8 deep, 40" per minute, climb milling, which the machine is built for

Scan from 1939

 

[DMF_TomB]

I'd like to thank TomB, Sfriedberg & Cal for their responses. I will need to do some more experimenting in the horizontal mode to get a better feel for the machine.
I had to get a ladder to get a better view of the motor nameplate and was able to confirm that it is 3hp. I don't have a backlash eliminator; as far as I know the backlash eliminator was only available on universal table mills.
When I first got the mill I tried climb milling ONCE ; and that was one time too many! I adjusted the gibs after my climb milling fiasco and have them a little on the tight side; I'll have to put an indicator on and test for movement like Cal suggests.
I'll have to send a couple of cutters out to get sharpened so that I will be able to learn the difference between sharp and dull.
Thanks for all the help, its nice to know the machine should be capable, and the issue is most likely operator error.

From the comments, I think I was going in the wrong direction, taking too light a cut when I should have been more aggressive. I just took a .100 cut after readjusting the speeds & feed without issue.

Am I correct that taking too light a cut and the cutter to rubbing caused the rumbling noise?

Mike

.
3 hp motor means often 1.5hp at the spindle. yes you might get 2 hp at the cutting tool end but usually motor is bigger than machine can handle and 1.5hp cut is probably all it can handle.
.
you could put a 50 hp motor on a machine but it does not mean it will not shake itself to pieces
.
similar to a Series 1 Bridgeport turret knee mill. you can have a 1.5 or 2 hp motor on it but i find when the cutting gets close to 0.75 to 1hp the vibration level starts going way up.
.
a wavy flute roughing cutter can help a lot. they cut more depth and width with less vibration

 

[Reeltor]

It certainly could, but other things are possible, too.

I needed to mill .400 deep across a piece of cold rolled, cutter took the cut like the steel wasn't even there. I did notice a slight noise when the cutter was in the cut. It's not loud, but it is there, How would I know if the noise is just the nature of the beast or if there is something I should check. What "other things" should I look at?

Mike

 

[DMF_TomB]

sorry but a 3hp machine and what looked like a big depth of cut going at hss toolng speeds 70 years ago is not enough now a days.
.
a big 6" dia face mill at 0.150" depth of cut going 50 inch per minute is 0.150" x 6 x 50 = 45 cubic inches per minute or about 56 hp in 1018 steel
.
your little 3hp machine can not handle modern carbide tooling in the larger sizes at higher speeds and feeds. it is not even close to capable.

 

[Reeltor]

sorry but a 3hp machine and what looked like a big depth of cut going at hss toolng speeds 70 years ago is not enough now a days.
.
a big 6" dia face mill at 0.150" depth of cut going 50 inch per minute is 0.150" x 6 x 50 = 45 cubic inches per minute or about 56 hp in 1018 steel
.
your little 3hp machine can not handle modern carbide tooling in the larger sizes at higher speeds and feeds. it is not even close to capable.

I don't follow you,

 

[Cal Haines]

I think he was talking about the machine in post #9.

Cal

 

[johnoder]

Here is another, my point again being they knew enough to let each tooth work as hard as possible - and they had also latched onto flood cooling via hood over cutter. Note SFM on this HSS cutter in steel ( Edit in better view of coolant hood)

Scan from 1913, the lads at CMM pushing the envelope on the relatively new HSS

http://img.photobucket.com/albums/v337/johnoder/MillPerformance1913.jpg

 

[Reeltor]

John, your comments are always welcome; they sure moved some metal!
I especially like the page with the coolant hood and will try to fab. something up for my VN, along with an outboard brace support to increase the rigidity of my setups.

 

[Mike C.]

Outboard support does wonders for the VN with its single round overarm. Had one on the 22L at the museum.

Sorry to have been gone for a while. WAY too much stuff going on and something had to give.

 

[Ohio Mike]

Here's what the support looks like

 

[Reeltor]

Here's what the support looks like
View attachment 131345

Ohio Mike,
Thank you for the photo, do the sweeping lines have any function, other than the cool factor?

Mike

 

[Ohio Mike]

Ohio Mike,
Thank you for the photo, do the sweeping lines have any function, other than the cool factor?

Mike

I don't think so, but it does have beautiful lines. I have to admit I haven't used it. It didn't come with the mill, I managed to snag it on eBay. A guy could fabricate one by machining a weldment, or have someone burn one out of a piece of plate.