What's new
What's new

What size 45 degree face mill for 2hp Bridgeport?

housedad

Aluminum
Joined
Oct 2, 2009
Location
NJ USA
I'm looking to get a 45 degree face mill for my Bridgeport. It has a 30 taper spindle. I want it for facing mild steel and some aluminum I don't forsee doing any major material removal with it, just primarily cleaning up. I have smaller indexable end mills for hogging, and a 2" Iscar 90 degree face mill for everything else.

I have fly cutters, but they are getting to be inconvenient.

Considering the expected use, could I reasonable get by with a 3" seht/sehw type cutter, or should I look for a 2-1/2 inch?
 
I'm looking to get a 45 degree face mill for my Bridgeport. It has a 30 taper spindle. I want it for facing mild steel and some aluminum I don't forsee doing any major material removal with it, just primarily cleaning up. I have smaller indexable end mills for hogging, and a 2" Iscar 90 degree face mill for everything else.

I have fly cutters, but they are getting to be inconvenient.

Considering the expected use, could I reasonable get by with a 3" seht/sehw type cutter, or should I look for a 2-1/2 inch?

.
1) 2hp motor figure 1hp available at the spindle
.
2) 1018 steel figure 1 cubic inch per minute takes about 1.0hp
.
3) 2" wide by 0.1 depth thats 0.2 cubic inch per inch of feed
at 20ipm feed thats 20x.2= 4hp needed
 
Face mills eat up horsepower almost just by looking at them. I say 2" tops. But mostly I'd use what you've experienced with your 2" 90 degree cutter and go from there, with the idea that a 45 will do a little bit more for less. Especially the high positive ones. Though they're not great on thin materials.

Dave
 
I use a 2.5" facemill with 45 degree inserts on my 2hp Bridgeport. It seems to do fine taking .100" cuts in mild steel.

.
cutting parameters is a science and its related to cubic inches per minute turned into chips. obviously if you go slower feed you use less hp.
.
power loss is typically 10 to 50% for small machines, got to due to how tight belts are, thickness of gear oil, etc. 2hp motor you get roughly 1.0 to 1.5hp at the spindle (depends what rpm it is set for) and the rest of the machine typically starts vibrating at max hp which is why they dont put a 5 or 10hp motor on the mill
.
1018 steel usually you get 0.8 to 1.6 cubic inch per minute per hp. depends on type of insert and the ipt feed rate
2.dia at 0.1 depth thats 0.2 cubic inch per inch of feed
.
roughly 0.2hp needed per every inch per minute feed. obviously if you go 5.0 ipm feed thats 1.0hp needed.
.
i run 2" facemills usually 20 to 60 ipm feed so thats it will use 4 to 12hp
with some positive rake inserts it could be 3 to 9hp either way only way could use on Bridgeport is go very slow or very low depth and width of cuts (which 0.1 is a low depth of cut)
 
I would think that, WITHIN REASON, the size of the cutter is more related to the size of the work, not of the mill. A 2.5" cutter will require a second pass on a 2.75" wide part while a 3" one will do it in one. If you are in a commercial shop, time is money.

Now, I am not just saying that bigger is better. There are other factors. If you are only going to have one such cutter, then do consider all of them. And if you almost never do any facing wider than, say 1.5", then either of your suggested sizes would be OK. Then, if you do a wide range of sizes, then you may want to consider two or even more cutters.



I'm looking to get a 45 degree face mill for my Bridgeport. It has a 30 taper spindle. I want it for facing mild steel and some aluminum I don't forsee doing any major material removal with it, just primarily cleaning up. I have smaller indexable end mills for hogging, and a 2" Iscar 90 degree face mill for everything else.

I have fly cutters, but they are getting to be inconvenient.

Considering the expected use, could I reasonable get by with a 3" seht/sehw type cutter, or should I look for a 2-1/2 inch?
 
Large diameter cutters will also amplify any tram issues you have. It may look flatter but many passes with a smaller cutter may actually be flatter. Think scraping.
Tipped sideways you will have a low center. Nod tipped will give you a tapered piece.
Sometimes it is nice just to make it look flat though. If you have a problem with surface finish from the back side dragging, tip the head a little.
On nylon jobs I do finish passes in that direction.

Dave
 
Most will run a 2 inch as old reliable and have a three to four inch for some light facing work. Anything under a 2 inch usually has a terrible tooth density so much time is spent cutting air.
One, two and three tooth facemills are not very nice in material removal or just the plain beating that takes place.
If I want flat I'll put in a 8 or 10 inch with many empty pockets. At that point it is a multi tooth flycutter not a face mill.
I'll also tram it with a very slight dish so that the back side does not touch. You do not want to do this will smaller diameter cutters.

This and it's bigger brother are quite decent for the money spent for a facing tool. I use one on a 10x54 B-port style and rate it as a solid okay.
Not stellar but very cost effective and as good as it gets in this standard design.
ZCC USA FACE MILL
Bob

Yes it is science but DMF is so way oversimplifying it with fudge factors that he has found or came up with and I tend to get wound up too tight when seeing such.
To his credit he does try to use an analytical approach and not just seat of the pants gut feel so I really should be nicer.
 
Most will run a 2 inch as old reliable and have a three to four inch for some light facing work. Anything under a 2 inch usually has a terrible tooth density so much time is spent cutting air.
One, two and three tooth facemills are not very nice in material removal or just the plain beating that takes place.

This and it's bigger brother are quite decent for the money spent for a facing tool. I use one on a 10x54 B-port style and rate it as a solid okay.
Not stellar but very cost effective and as good as it gets in this standard design.
ZCC USA FACE MILL
Bob

Yup^^

The mill you linked to looks similar to valenite & wesson offerings in the 80’s Bob! I used to call them whisper mills, larger ones you mounted with leather gloves cause they were SHARP! :eek:

I have some inserted shoulder & face mills for the R8 sized machines but to be honest I can’t remember anything that worked better than the 1&½ to 2&½ HSS shell mills for VERY quietly removing metal & keeping the little motors warm - but still happy. They DO have very good tooth density (fine pitch in mill talk)...

I see Maritool even offers them here → General Purpose High Speed Steel Shell Mills - MariTool

Matt
 
1) i have used Bridgeports for about 4 decades now and many a time have i stalled motor cause i was taking too much at too high a feed. obviously if hand feeding you go slower feed if you notice motor slowing down
.
2)30 taper is better than a R8 as i have also damaged the set screw key that keeps R8 collet from spinning. and many a time i have had head go out of tram cause i overloaded or broke even a 1/2" end mill
.
3) my experience is a roughing end mill corn cob type is more energy efficient or cuts more cubic inches per minute per hp with less vibration chatter. a 1" roughing end mill again if removing 0.2 cubic inches per minute per inch feed tends to use less than 0.2hp per inch feed so if going 5 ipm feed its under 1 hp.
....obviously can use a bigger end mill like a 1.75" roughing end mill but if you tried 1.7" depth at 1.7" width of cut thats 2.9 cubic inch per inch feed so even a slow 3 ipm feed thats 5.7 - 8.7hp required
.
4) my experience on a bridgeport their a reason they dont put bigger motor on them. they vibrate or chatter or shake too much when near hp of the motor they normally put on them. .....same cutting parameters using 1.0hp at spindle and bridgeport is vibrating, chattering, etc on a bigger mill it will be much quieter.
.
math is one of those laws of the universe. sure some dont believe the laws of the universe apply to themselves but they do. doesnt matter whether you want to believe in them. they are what they are.
.
there is a hp to cubic inches turn into chips ratio. sure it varies with cutter type, sharpness, ipt feed rate. usually 1018 steel is stated at 0.8 cubic inch per minute per hp, sure it can get up to 1.6 with some cutter types and cutting parameters but it always in the range of 0.8 to 1.6 cubic inch per minute per hp. sure some use 1.0 to get a rough calculation
.
its like apprentice wants to buy a 1" dia carbide insert drill thats .78 cubic inch per inch depth if drill manufacturer recommends 30 ipm feed thats 23.5hp required. obviously on a 5hp machine you aint going to be able to run it at the recommended settings. kind of want to know that before you buy it. you can buy a carbide insert facemill for a bridgeport just realize it cannot run it any where near recommended max settings
 
To me, everything over ~3/4 you are not doing max material removal. I would rather use my hands and ears to set the feed with a 3/4 end mill to rip off some material than try to push the horsepower through a big tool. I have some round insert[rotary IIRC] face mills about 2 inch diameter that can take a chip on my R8 3HP Lagun, but it is way more rigid[trammed once a decade, or when I run the quill into the vise]

Newer technology can work in older tools. Almost 30 years ago, working a contract job. Picture a row of guys at manual bridgeports cutting steel, squeek squeek squeek. Had a chunk of tool steel I needed to rip down. Brought an inserted end mill in from my shop.


I wish I had a picture of their faces when I wound the spindle up and sent a shower of glowing metal chips off the machine.

Fun
 
been my experience even if you had more hp, if you do a lot of roughing you have high enough cutting forces head wont stay in tram. worse if when tram off moderate amount but not immediately obvious. i used to check tram every day cause bridgeport kind of flimsy and often roughing pushed it out of tram
.
sure if using facemill and taking 0.030" or less depth of cut you can use it but same facemill might easily handle 0.150" depth of cut on a bigger machine at much higher feed rates. usually facemill goes 20 to 40 ipm feed not 2 to 4 ipm
 
I'm with Bob on this one. I never had to run a 2" facemill at 2-4 IPM on Bridgeports in any shop I was in. They aren't stiff machines by any means, but every one I ran (2HP for the most part) could manage a .100" depth of cut at 15 IPM (max feed speed of the power feeds we had) using a 2" SEKN insert cutter as long as I didn't try to approach full cutter width. That was my standard roughing cut on a Bridgeport. Maybe get some better Bridgeports?

And to be honest, if you need to really hog off some steel, you shouldn't be using a Bridgeport anyway...

Get over to a mill with some rigidity and do it the right way. Even using a corncob rougher on a Bridgeport is a waste of time if you have any large amount of material to remove. And if you don't have much to remove, who cares if it is at lightning speed anyway?
 
Another issue to consider: taking heavy cuts with a large face mill generates enough force to knock the machine out of tram. I settled for a 3" high positive 45* cutter for my 3hp. machine.
 
Thanks everyone for the help. I went with the 2.5 inch unit from Glacern. Not able to take deep cuts, but Wasn't looking for this to hog with, anyway. The mill is a Series II Special, but it still has the ram and head of a standard bridgeport. I will watch the tram and see what it can do on this machine.
 
1) i have used Bridgeports for about 4 decades now and many a time have i stalled motor cause i was taking too much at too high a feed. obviously if hand feeding you go slower feed if you notice motor slowing down
.
2)30 taper is better than a R8 as i have also damaged the set screw key that keeps R8 collet from spinning. and many a time i have had head go out of tram cause i overloaded or broke even a 1/2" end mill
.
.
4) my experience on a bridgeport their a reason they dont put bigger motor on them. they vibrate or chatter or shake too much when near hp of the motor they normally put on them. .....same cutting parameters using 1.0hp at spindle and bridgeport is vibrating, chattering, etc on a bigger mill it will be much quieter.
.
math is one of those laws of the universe. sure some dont believe the laws of the universe apply to themselves but they do. doesnt matter whether you want to believe in them. they are what they are.

hmm.. math is one of the laws of the universe.. ok Tom how about THIS math, some don't have the money or space to buy 50HP 30,000 lb machines! just be reasonable and don't push the crap out of a BP, and the machine you have can often get the job done, THAT'S the math a lot of us deal just fine with.
 
Say... couldn't you make an adapter out of billet aluminum ( for weight) and have R8 on the end and a socket for50 mill taper on the end? That way you could use a surplus 8 or 10 inch face mill of of one of those old horizontal mills that nobody wants!!
 
My experience is that on weaker machines you cannot actually use facemill for steel. Inserts need a minimum DOC and if lower, they rub and break and chatter.
Look for the HSS world.

For aluminium, 2" - 3" should work nice.
 








 
Back
Top