[How-To] Speeds and feeds (general advice)

[peterh93]

Hi guys new to the forum and this is my first post so bear with me.


TLDR: Help with speed and feeds of a 4 insert cutter on a bridgeport milling machine on low alloy steel

Looking for some advice with speeds and feeds and general help with using a bridgeport milling manchine.

Advice such as how to tell how well material is cutting (noise, vibration, heat, finish etc)

What tools are best for what job in general? Like material removal, Finish, precision etc

So my problem that im asking about is im currently machining 16x low alloy steel blocks im removing material ready for its next stage of grinding attached is a video that i think will help show the cutting at the moment better than i could describe....

Edit: video wont upload but yea my problem is a lot of heat is being generated and a lot of noise (not allowed to use coolant) and i don't know if this is cutting correctly or not?

Cutter is a 4 teeth (4 inserts)
Cutter speed: 550
Traverse speed:100 (now on 125)
High range and high speed (switches on the head)

Picture of blocks finish in vice is with brand new tips on the cutter. Picture in my hand is a finish after the cutters done one block.

Thanks in advance for any help

 

[Eddyde]

Hi welcome to HM.

It can be tricky to get a good finish with carbide tooling. Depth Of Cut is a factor, try increasing it, if too light, the tool can't get a good bite and will tend to have more of a scraping than a cutting action. High Speed Steel generally gives a better finish, particularly in softer, gummier metals. This is because HSS can attain a sharper edge than carbide.
Feeds and speeds are not super critical for HSS, they are more important with carbide and each insert will generally had an optimum DOC and Surface Feet Minute, that you can use to determine the best F&S. But there is a range and it doesn't always need to be optimum.

 

[peterh93]

Hi eddy thanks for your reply

The finish isnt really important to me but i thought it would be a good indicator of how the cutting is going, my current depth of cut is 0.5mm should i increase this?

 

[pontiac428]

When working with carbide, I work backwards to my final dimension to ensure I get enough depth of cut on the final pass. So if .050 is to be removed, I go .010 first, then .020 to verify the finished cut is indeed .020, make any adjustments needed, and make the final cut which would be in the neighborhood of .020. The last cut is always a full step. With HSS, you can make two full steps then clean up what's left, carbide won't allow that, it wants a full bite. My .02 cents for your .020 sound good?

Edit: No need for carbide on low alloy anyway, unless that's the tool you've got. A nice single point HSS fly cutter will allow for very fine finish passes with just a slight hand-honed radius on the tool.

 

[Winegrower]

Plus, check your mill tramming…it looks like there is a leading to trailing edge difference.

You will want to make a full pass across the part for the best finish, not stopping mid-sweep.

The chips look acceptable to me.

 

[MrCrankyface]

In my experience some insert cutters generate very high cutting forces, making it sound terrible as it's taking up and releasing slack in the head and gearbox etc. This quickly gets worse as the diameter of the cutter grows.
That generally makes it really hard to tell if it's cutting good/bad and if it's a feed/speed problem or insert problem, at least from sound.
I don't see a mention of the cutter head diameter and also what unit is your traverse speed in?

To my eyes it looks like the metal is tearing rather than cutting(both the specks and burrs) but could be exaggerated from being a high-res photo.
Assuming your cutter is around 2" diameter I think you're pretty close to the right feeds and speeds.
I would probably try upping both rpm and feed, if that doesn't make it better, see how the finish looks with a lower feed(if that removes some of the radial lines)
The inserts looks like they should handle a 0.5mm DOC but only way to find out is to take 1mm DOC and see if it sounds and looks better or worse.
In general I find that you need to run inserts fast in both feed and RPM and take a deep enough cut so the full nose radius is engaged.
If you take even deeper cuts you might start running out of machine stability on these smaller machines and on shallower cuts the insert won't work properly.

Just to give an example of what usually works for me on a very slightly heavier machine.
I use a few of these 1604 inserts, head is around 30mm in diameter and I run it at ~1100RPM in steel.
The most I usually dare feed from a stability standpoint is then 500mm/s but it definitely wants to travel even faster.
With this I've found 1mm to be some kind of sweet spot on my machine, more will cause a lot of slamming from cutting forces and less produces horrible finishes.

 

[peterh93]

When working with carbide, I work backwards to my final dimension to ensure I get enough depth of cut on the final pass. So if .050 is to be removed, I go .010 first, then .020 to verify the finished cut is indeed .020, make any adjustments needed, and make the final cut which would be in the neighborhood of .020. The last cut is always a full step. With HSS, you can make two full steps then clean up what's left, carbide won't allow that, it wants a full bite. My .02 cents for your .020 sound good?

Edit: No need for carbide on low alloy anyway, unless that's the tool you've got. A nice single point HSS fly cutter will allow for very fine finish passes with just a slight hand-honed radius on the tool.

Thanks for helping unfortunatly this is the only cutter thats big enough to do the block in one full pass (well nearly). So how much of a cut shoukd i be taking to get a proper bite?

 

[peterh93]

Plus, check your mill tramming…it looks like there is a leading to trailing edge difference.

You will want to make a full pass across the part for the best finish, not stopping mid-sweep.

The chips look acceptable to me.

What is mill tramming? And yes ive not been fully passing as im taking anouther cut striaght afterwards and then the part goes for grinding so the finish isnt an issue for me

Thanks for your help

 

[peterh93]

In my experience some insert cutters generate very high cutting forces, making it sound terrible as it's taking up and releasing slack in the head and gearbox etc. This quickly gets worse as the diameter of the cutter grows.
That generally makes it really hard to tell if it's cutting good/bad and if it's a feed/speed problem or insert problem, at least from sound.
I don't see a mention of the cutter head diameter and also what unit is your traverse speed in?

To my eyes it looks like the metal is tearing rather than cutting(both the specks and burrs) but could be exaggerated from being a high-res photo.
Assuming your cutter is around 2" diameter I think you're pretty close to the right feeds and speeds.
I would probably try upping both rpm and feed, if that doesn't make it better, see how the finish looks with a lower feed(if that removes some of the radial lines)
The inserts looks like they should handle a 0.5mm DOC but only way to find out is to take 1mm DOC and see if it sounds and looks better or worse.
In general I find that you need to run inserts fast in both feed and RPM and take a deep enough cut so the full nose radius is engaged.
If you take even deeper cuts you might start running out of machine stability on these smaller machines and on shallower cuts the insert won't work properly.

Just to give an example of what usually works for me on a very slightly heavier machine.
I use a few of these 1604 inserts, head is around 30mm in diameter and I run it at ~1100RPM in steel.
The most I usually dare feed from a stability standpoint is then 500mm/s but it definitely wants to travel even faster.
With this I've found 1mm to be some kind of sweet spot on my machine, more will cause a lot of slamming from cutting forces and less produces horrible finishes.
View attachment 435732

Hi thanks for the help mr cranky face i upped the rpm to 700 from the 550 i was on and the cutting didnt seem to get any better although im now producing new swarf on top of the chips already produced ( see attaced pic) and the noise from the gearbox and taking up and relases slack has become a little better (thankyou for explaining that by the way as i have no idea if them nosies where acceptable hence leading me to this forum).

The cutter is just over 2 inches in diameter from tip to tip.

I chose this cutter as it was the biggest diameter therefore removing nearly all the material of the face of the block in one pass.

Could you send me a link to your cutter? And maybe a bigger diameter one as to not have to do multiple passes on my block?

Im hesitant of going any faster on me feeds and speeds as it sound awful as it is on the bridgeport series 1 and i dont fancy damaging the cutter, the block or the miller...

My trav speed units is mm per min and its currently on 125

Thanks again for you help appricate it!

 

[MrCrankyface]

Whilst not "professional" I really like this calculator because it's easy to use:

Speeds & Feeds

The premier source of tooling, parts, and accessories for bench top machinists.

littlemachineshop.com

Just input your numbers and you get a ballpark figure to start from.
Both from what the calculator is spitting out and my "gut feeling", I would say you're feeding way too little for that RPM, but you need that RPM to keep the cutters happy, hence why inserts can be problematic.
They need to be at a high enough RPM and high enough feed to get a good bite into the material, but this will result in such a high material removal rate(MRR) that your machine isn't sturdy enough and things could get damaged or result in an even worse finish.
Think of it as towing a yacht with a scooter and expecting the same result as with a truck.

I haven't tried cutter heads in the area 40-120mm but I know my 140mm one makes one hell of a racket if I have all teeth in and run it at the "correct" feed(which is scary as heck).
My "solution" there has been to remove some teeth so I can still run a high enough RPM and with less feed, challenging the machine less.
Basically turning my 12 insert cutterhead into a 3, 2 or even 1 insert cutterhead, reducing the "necessary feed" from an insane 2452mm/min to a more reasonable 204-613 mm/min.
Basically what you're gaining from having several inserts is time. You can feed into the material faster by having more teeth engaged at all times, if your mill is sturdy enough.
If your machine is not sturdy enough and you back off on feed, you're only wasting inserts and cut quality.
IMHO I think we're talking multi-tonne machines to really push these kind of cutters into their comfort zone.

I believe this is the endmill I'm mostly using:
shorturl.at/rBCV6 (BAP400R C25-30-150)
Works well at 0.5-2mm DOC for me, in typical steel usually 800-1200RPM and up to 600mm/min feed depending on the setup.
This is in cast iron(I have shortened the endmill a bit to lessen stick out):

TLDR thoughts:
1. Try increasing feed much more to get a good bite, if it sounds bad/vibrates too much etc try removing cutters to basically make it into a fly cutter and you can back off the feed.
2. Using a smaller cutter(like the 30mm one) would produce less cutting forces and allow you to climb-cut around the perimeter, removing a lot of the burrs you seem to get. Granted this is maybe more of a PITA on a manual machine.
3. Make a dedicated fly cutter with inserts, I made one for DCMT lathe inserts, works great and produces quite small cutting forces. Not a mass-remover, more of a finisher.

Edit:
Mill tramming is making sure your head is perfectly perpendicular to your X and Y axis. To exaggerate, you don't want your cutter to be angled 45* off as this will cut ovals into your surfaces, not flats.
Blondihacks got a bunch of good intro videos: