What's new
What's new

Is this a prank? Mitee-bite ID expansion clamp recommended feed rates...

xnewmanx

Aluminum
Joined
May 19, 2016
The recommended machining practices for the clamps direct fdrom mitee-bite's site:

Aggressive material removal is not recommended when machining clamps to size. Suggested machining practice is to spiral down with a .500" end mill by conventional milling 0.020" off the desired clamp diameter at 400 SFPM and .001" per flute and .02 depth per trip around. Finish final diameter at 700 SFPM using same .001" per flute feed and .250" depth and climb mill.

Using these parameters it's going to take over 10 hours per clamp and I have to do a dozen of them... Anyone have any real world reccomendations?
 
Is your clamp ten feet in diameter? Or a 300 RPM spindle? Those are conservative feeds and depths but, I don't see more than a few minutes. 400 SFM on a 0.5" endmill is 3055 RPM. 3055 x 0.001 per tooth on a three-flute? 9 IPM. I'd probably round those at 10 IPM and 3,000 RPM. 0.020 per lap of depth? Again, how big a clamp are we talking about?
 
.02" radial sounds right but axial too is :nutter:. I would go full axial and around .02" radial depending on how it sounds. How much metal do you need to remove? If you have a bunch of metal to remove maybe rough with a corncob mill to reduce the cutting forces.
 
Is your clamp ten feet in diameter? Or a 300 RPM spindle? Those are conservative feeds and depths but, I don't see more than a few minutes. 400 SFM on a 0.5" endmill is 3055 RPM. 3055 x 0.001 per tooth on a three-flute? 9 IPM. I'd probably round those at 10 IPM and 3,000 RPM. 0.020 per lap of depth? Again, how big a clamp are we talking about?


It's about 3 inches in diameter and about 1" in height. I have to remove about .5" per side.

.5 per side / .020 per pass = 25 stepovers
1 height / .020 per rev = 50 stepdowns

so 1,250 passes per clamp. Total machined distance for one roughing op is almost 12,000 inches.
 
Yeah, I was picturing maybe 0.25" depth of total cut on a sub 1-inch diameter. Agree that the radial engagement could go up quite a bit. The depth is going to wear the corner of the endmill but, they're clearly trying to avoid the side force on the clamp.
 
It's about 3 inches in diameter and about 1" in height. I have to remove about .5" per side.

.5 per side / .020 per pass = 25 stepovers
1 height / .020 per rev = 50 stepdowns

so 1,250 passes per clamp. Total machined distance for one roughing op is almost 12,000 inches.
Although I do agree that the recommendations sound conservative, it sounds more like they want you to do one ramp at .02 per revolution and leave .02 for the finish pass, not take .02 radial on each ramp.
 
Although I do agree that the recommendations sound conservative, it sounds more like they want you to do one ramp at .02 per revolution and leave .02 for the finish pass, not take .02 radial on each ramp.

I was trying to read it another way and couldn't really think of anything i was missing. I suppose that's one explanation.
 
Although I do agree that the recommendations sound conservative, it sounds more like they want you to do one ramp at .02 per revolution and leave .02 for the finish pass, not take .02 radial on each ramp.
That's how I read it. When it says ".02 off" I took that to mean go at it full width if necessary but just leave a .020" finish pass.
 
Do people actually leave 0.020" finishing stock allowance on a mill when cutting steel?

Makes sense on a lathe due to the insert corner rad. Makes no sense on a mill unless it's aluminum, which these are not. Not gonna hit size consistently with that much stock allowance. An edge prepped carbide endmill has a corner radius of about 0.001" on the cutting edge. A finishing endmill often has no edge prep (debatable whether that's good or bad). So the finishing stock allowance should me more like 0.002". At 0.020", a spring pass is mandatory.
 
Do people actually leave 0.020" finishing stock allowance on a mill when cutting steel?

Makes sense on a lathe due to the insert corner rad. Makes no sense on a mill unless it's aluminum, which these are not. Not gonna hit size consistently with that much stock allowance. An edge prepped carbide endmill has a corner radius of about 0.001" on the cutting edge. A finishing endmill often has no edge prep (debatable whether that's good or bad). So the finishing stock allowance should me more like 0.002". At 0.020", a spring pass is mandatory.
This is exactly why I was thinking they were talking about stepover not finishing. Seemed like a ton to me. I usually leave .003-.005.

But also I don't know what I'm doing.
 
Seems a little crazy they would recommend to go that slow. I would increase all those parameters personally.

Even more crazy is to recommend using a 1/2" tool for such a light cut. A smaller tool would run higher rpm which means faster feed rate plus lower tool costs.
 
Remember guys, he is trying to machine the clamp. He isn't looking for production.
ID-Clamp-1-e1626191269780.jpg
 
OK, I'll bite:

it sounds more like they want you to do one ramp at .02 per revolution and leave .02 for the finish pass, not take .02 radial on each ramp.

That's how I read it. When it says ".02 off" I took that to mean go at it full width if necessary but just leave a .020" finish pass.

I have absolutely no friggin' idea how you two fellas understood the initial post, reading:
milling 0.020" off the desired clamp diameter at 400 SFPM and .001" per flute and .02 depth per trip around.

I know, I may have had 2 beers, but come on, what did I miss???
How in the living hell does anyone interpret that idiotic verbiage as: Leave .02 for finish depth!

Is Mitee-Bite now owned by a Chinese company, or they just employ the same folks who write the Fanuc manuals?
 
Last edited:
OK, I'll bite:





I have absolutely no friggin' idea how you two fellas understood the initial post, reading:


I know, I may have had 2 beers, but come on, what did I miss???
How in the living hell does anyone interpret that idiotic verbiage as: Leave .02 for finish depth!

Is Mitee-Bite now owned by a Chinese company, or they just employ the same folks who write the Fanuc manuals?
Because it says to run at .020" off the DESIRED clamp diameter. It doesn't say to step in .020" at a time from the OD until you get there. Just to clarify, the .020" finish depth is diametric, so really only leaving .010" per side.
 
I would say that their wording is not great, but not quite chinese translation bad.

You'll get people like the op who read it as "this thing can barely take a cut" once in a while but 95% would get the idea.

I can pretty much guarantee that someone at mitee bite had a support phone call where someone was complaining their clamp wasn't working when they cut it. After some back and forth, they probably realized the person who cut the clamp just went right for the diameter they were trying to cut, maybe even didn't make a spring pass. The thing was probably all kinds of out of round and probably had places where it dug in, etc.

Just writing this, I'm struggling to think how to write it that everyone would agree with, spending just about 1 minute thinking about it.

I would say I think ramping down .020" in z every cut is a poor way to suggest cutting it? I'd be ramping radially around in a spiral, not a downward helix.

Edit: after reading again, I'm not even sure when they say ".020" depth per trip around" that they mean z depth? I almost wonder if they mean radially?

Someone come up with an illustration!
 
I would make a flat disk (1/4 ?)thick that is the same target diam as the finish diam of the clamp
Secure it to lock "fingers" from moving
Rough it aggressively to 020 over final target diam
Remove disk
Finish to needed diam
 
Just to clarify, the .020" finish depth is diametric, so really only leaving .010" per side.

Man, I really need to go back to school and brush up on my English.
Forget the wording ( depth vs. engagement vs. side ), just where did the diametric definition come from?
Taking a .020 deep cut means taking off .020 from whatever the hell you're cutting.
If that sumbitch happens to be a diameter, and you're taking a .020 deep cut, your diameter will be .040 smaller/bigger, and yet, you're still taking a .020 deep cut.

So what happens if you're making a flat on that otherwise round Mitee-Bite clamp? You're gonna do mental math and suffer over how it is measured to figure out whether to take .010 per side or .020 per side?
 
Man, I really need to go back to school and brush up on my English.
Forget the wording ( depth vs. engagement vs. side ), just where did the diametric definition come from?
Taking a .020 deep cut means taking off .020 from whatever the hell you're cutting.
If that sumbitch happens to be a diameter, and you're taking a .020 deep cut, your diameter will be .040 smaller/bigger, and yet, you're still taking a .020 deep cut.

So what happens if you're making a flat on that otherwise round Mitee-Bite clamp? You're gonna do mental math and suffer over how it is measured to figure out whether to take .010 per side or .020 per side?
The diametric part comes from when it says " milling 0.020" off the desired clamp diameter". The instructions are assuming you are milling a circular feature from the way they are worded and telling you to stay off of a diameter by a certain amount, reading "off" as "away from". If I said my diameter is off .020" to the big end, wouldn't that mean there is .010" left over per side to remove? The part of the instructions that says "and .02 depth per trip around", is axial depth which is indicated by the beginning of the sentence stating "Suggested machining practice is to spiral down.......and .02 depth per trip around". This is further reinforced when the finish pass says to take a depth of .250". It's not an English problem, it's a context issue.

I whole-heartedly agree that it is one of the most poorly worded instructions for how to cut something I have seen, but I also think that trying to prove how poorly worded it is is blinding some peoples comprehension of the instructions.
 








 
Back
Top