What's new
What's new

Best toolholding system for fine surface finish (and hard-milling)? CAT40

aarongough

Stainless
Joined
Oct 27, 2014
Location
Toronto, Canada
Hey guys!
This weekend I am going to be rebuilding my VMC (Fadal VMC10) with the goal of chasing better surface finishes for making my product... I will be replacing the spindle, XYZ ballscrews, couplers and thrust bearings all with new components to replace the 20 year old worn out ones.

The machine is currently in poor shape. Spindle taper is bell-mouthed, has low drawbar pressure, as well as 0.0016" of runout. Ballscrews are also in poor shape with around 0.0015" of backlash on each axis. Obviously surface finish as-is is sub-par.

Right now I am 3D contouring to finish the surface of my blades. Using a 1/4" 4 flute carbide TiAIN coated endmill with 0.060" corner radius, running 7500RPM and 50IPM in a short gage length ER25 holder. Material is annealed A2 tool steel. The results I'm getting are poor and I know I can do a lot better. Example of current surface finish shown here: (ignore messed up bevel from fixturing issue!)



My goal with the rebuild and the desire to re-tool is to drastically improve the surface finish that I'm able to achieve straight off the VMC. I don't particularly care if cycle time goes up, I just want to eliminate as much hand work as possible as it's a huge source of inconsistency.

Early next year I will be looking to move to hard-milling to continue chasing better surface finishes while also simplifying my process...

Ok long winded intro is over... My question is: what toolholding system(s) should I be looking at?

Currently I'm using short gage length ER25 holders from Maritool (which are great!) but I know there are other systems that tend to have lower runout. The guys at Maritool have CAT40 SK collet holders that look like they would be better, but what is the best system I can get?

I know the guys that do hard-milling on molds use a lot of shrink-fit tooling, is that what I should be looking at as well?

Note that I don't need long gage-length tooling... I'm currently using 1.85" gage length ER holders with stub-length endmills and that gives me plenty of reach, so long toolholders are not necessary.

Any and all input greatly welcomed, thanks guys!

-Aaron
 
If you'd like the lowest runout and best current tool holder that I know of, the Albrecht Uberchuck collets are amazing. best runout rating, extremely rigid, fantastic grip strength, without the associated issues of shrink fit or hydraulic tool holders.

http://www.walterhammond.com/storefrontContent/attach/files/pdf/albrecht/albrecht_full.pdf

three different formats, APC-20 being the most practical for most uses (that's what we're using, in HSK spindles). 1/8-3/4" (20mm) capacity with typical sizes of collets to suit standard and metric tool shanks.

up to 1.25"/32mm tool diameter with the APC-32.
 
Honestly, I've done some pretty crazy finishes with side lock (set screw) style end mill holders. If they are quality with offset ground bores the runout is on par with most other style holders. I've also had good results with hydraulic holders for light finishing, the runout is even better and they tend to have a dampening effect.

Shrink holders are hard to beat for longer gauge length but for short stuff like you are doing I think the other options are right there.

You're on the right track with addressing the other issues with the mill. Taper and thrust bearings have a much bigger impact on finish than any high quality holder.
 
Honestly, I've done some pretty crazy finishes with side lock (set screw) style end mill holders. If they are quality with offset ground bores the runout is on par with most other style holders. I've also had good results with hydraulic holders for light finishing, the runout is even better and they tend to have a dampening effect.

Shrink holders are hard to beat for longer gauge length but for short stuff like you are doing I think the other options are right there.

You're on the right track with addressing the other issues with the mill. Taper and thrust bearings have a much bigger impact on finish than any high quality holder.

My main concern with using side-lock holders is that none of the tooling I'm using has flats on them, and I'm not really setup to grind the flats here, so I'd be worried about tools pulling out or shifting... I've heard of people running smaller tools (like 1/4") without flats but I gotta admit that makes me a bit nervous.

I've got some nice Maritool side-lock holders here in the correct sizes, I should give them a shot at the least!
 
If you'd like the lowest runout and best current tool holder that I know of, the Albrecht Uberchuck collets are amazing. best runout rating, extremely rigid, fantastic grip strength, without the associated issues of shrink fit or hydraulic tool holders.

http://www.walterhammond.com/storefrontContent/attach/files/pdf/albrecht/albrecht_full.pdf

three different formats, APC-20 being the most practical for most uses (that's what we're using, in HSK spindles). 1/8-3/4" (20mm) capacity with typical sizes of collets to suit standard and metric tool shanks.

up to 1.25"/32mm tool diameter with the APC-32.

That system looks really interesting... Very clever mechanism!

Are you using the uberchuck for hard milling?
 
I would say getting the spindle reworked would gain you alot more benefit then any new tool holder because a new tool holder will not eliminate that. If your using a rough then finishing strategy, your finish pass will have very little tool load. So a fancy tool holder is over kill. Corochucks and such are to over come pull out which you are not generating. Do your Z axis ball screw as it will allow the tool to fall into the piece. Most cnc control systems have ways to overcome backlash, not knowing your specific platform I can not offer much insight.
 
I second the side-lock holders Aaron. A few other things to consider.
First, with the tooling.
It doesn't take much of a flat to help keep an end-mill from moving in a side-lock. Get a diamond-wheel, and grind your own flats.
You are not spinning fast enough to be overly concerned with balance. Grind an .125-.200 wide flat on the shank, and tighten the screw up good and snug.
This would be my first step.
The next thing I want to mention, you may not like! LOL
If you can tilt the part (your knife blade), so that you are cutting farther from center of the tool, you will find instant positive results.
I know you have a lot of time in that fixture! And, you would have to pretty much start over with your programming.
But, if you can tilt that surface up, you will get a much better finish.

Using 4-flutes on that very shallow surface is kind of a waste of two flutes. You would be better off with a 2flute.
And, down at the very bottom of a ball end-mill, your SFM is very very low. Raising SFM will greatly improve surface finish.
And the only way to do it if your already at max RPM, is get up on the side of the tool. The flute geometry is better up on the side as well.
Tilt that blade up!
 
I would say getting the spindle reworked would gain you alot more benefit then any new tool holder because a new tool holder will not eliminate that. If your using a rough then finishing strategy, your finish pass will have very little tool load. So a fancy tool holder is over kill. Corochucks and such are to over come pull out which you are not generating. Do your Z axis ball screw as it will allow the tool to fall into the piece. Most cnc control systems have ways to overcome backlash, not knowing your specific platform I can not offer much insight.

Yeah, as I said in the intro I will be replacing the spindle, as well as ballscrews on all axes... The control (Fadal CNC88HS) has backlash comp built in, but I'm sure different areas of the screw are worn unevenly and the control can't compensate perfectly, so new ballscrews are the plan.

I use two identical 1/4" endmills during the process. One for roughing, one for finishing. Once the finish tool wears I move it to the rougher position and put a new tool in the finisher spot... I'm only looking to replace those two toolholders... The ER holders seem to be working very well for all the other operations.
 
That system looks really interesting... Very clever mechanism!

Are you using the uberchuck for hard milling?

No hard milling here, we use the Uberchucks for their low runout and dampening for high RPM aluminum sheet cutting (24K RPM routers up to half inch thicknesses). perfect for fastest cutter change too, since the sealed collet can stay in the holder and just the tool drops out when loosened by the side locking screw (which drives an internal worm gear action)

I would not hesitate to use this system on a quality VMC, it really blows ER collets out of the water (I've been using ER16/20/25/32/40 for a decade and trust them, but I know their limits and distrust most operators to treat them with adequate care to ensure lasting accuracy and lifespan)
 
I second the side-lock holders Aaron. A few other things to consider.
First, with the tooling.
It doesn't take much of a flat to help keep an end-mill from moving in a side-lock. Get a diamond-wheel, and grind your own flats.
You are not spinning fast enough to be overly concerned with balance. Grind an .125-.200 wide flat on the shank, and tighten the screw up good and snug.
This would be my first step.
The next thing I want to mention, you may not like! LOL
If you can tilt the part (your knife blade), so that you are cutting farther from center of the tool, you will find instant positive results.
I know you have a lot of time in that fixture! And, you would have to pretty much start over with your programming.
But, if you can tilt that surface up, you will get a much better finish.

Using 4-flutes on that very shallow surface is kind of a waste of two flutes. You would be better off with a 2flute.
And, down at the very bottom of a ball end-mill, your SFM is very very low. Raising SFM will greatly improve surface finish.
And the only way to do it if your already at max RPM, is get up on the side of the tool. The flute geometry is better up on the side as well.
Tilt that blade up!

Hey Wheelie!
I'm actually not using ball mills! :) I learnt the hard way what you mean about SFM reducing to near zero near the center and smearing the finish... So instead I got the guys at Maritool to make me some awesome stub-length corner radius endmills (bull-nose endmills). That way I can cut with the corner rather than the center and keep my effective SFM up... I believe that should avoid the need for tilting the part?

I will definitely have to try out my side-lock holders by the sounds of it! I've actually had them sitting here in the box for a while and have never used them...

-A
 
Why are you using such a small corner radius? A 1/4 ball or even a 1/2 ball will net you a better finish and allow you to increase your step over. You could always come back and pick the corner with the .06r
 
Never mid I see your reasoning. But I think tilting the part and going to a ball would be a huge advantage.
 
Why are you using such a small corner radius? A 1/4 ball or even a 1/2 ball will net you a better finish and allow you to increase your step over. You could always come back and pick the corner with the .06r

I've used ball mills in the past and surface finish was worse... Because the part is on a relatively shallow angle you end up cutting only with the very center of the tool... Stepover with the corner radius tool is much larger for same surface finish than with a ball mill from what I've seen. I'm running the tool down the bevel as opposed to across which allows me to present the tool to the work with a large apparent curvature..

EDIT: never mind, just saw your follow up post!
 
Why are you using such a small corner radius? A 1/4 ball or even a 1/2 ball will net you a better finish and allow you to increase your step over. You could always come back and pick the corner with the .06r

Already been said... Shallow angle...

I've got one part I run, 1.5 degrees on one side, 7 degrees on the other... Granted surface finish on this one doesn't mean shit, but I contour it with
a 2" facemill with .030 rad inserts. A bUll nose is going to win day in and day out on a shallow angle.

Edit: disregard.. Me too.

Aaron.. On the grinder thing and making flats... It DOES NOT have to be a fancy looking thing like a Weldon Flat.. All you need is something
flat.. Some type of green wheel on a regular old bench grinder works, but in a pinch even a shitty Harbor Freight or Lowes cheap POS grinding
wheel will get you a bit of a flat, and that is all you need.... You DO NOT need much, especially on a small endmill that isn't moving pounds of metal
a minute. You could probably even do it quick and easy with a dremel tool, and if you pushed, you might even be able to get enough on a belt sander.
 
Stand them up so the primary angle is vertical and 3D Contour the primary along the presharpened edge. I stopped surface milling my primaries and most of my swedges a long time ago and never looked back! Cut my cycletime from 15-20mins per side down under 2mins per side including roughing and finishing, using 1/2" off the shelf endmills for everything. I leave a solid tab along the edge to support the second side so I don't have to build up a supporting surface for the second side since the first primary is already cut. You can grind the tab off or lay them back flat and mill them off, which is how I've been doing it. You'll be sharpening that edge anyways so it doesn't make much difference how you do it.

I'm currently surface milling soft jaws at different angles for different primaries, but since all your blades are the same it would be super easy to make some dedicated fixtures at your primary angle and be done with it. Shoot me a DM on IG if you'd like to see some pics!
 
Stand them up so the primary angle is vertical and 3D Contour the primary along the presharpened edge. I stopped surface milling my primaries and most of my swedges a long time ago and never looked back! Cut my cycletime from 15-20mins per side down under 2mins per side including roughing and finishing, using 1/2" off the shelf endmills for everything. I leave a solid tab along the edge to support the second side so I don't have to build up a supporting surface for the second side since the first primary is already cut. You can grind the tab off or lay them back flat and mill them off, which is how I've been doing it. You'll be sharpening that edge anyways so it doesn't make much difference how you do it.

I'm currently surface milling soft jaws at different angles for different primaries, but since all your blades are the same it would be super easy to make some dedicated fixtures at your primary angle and be done with it. Shoot me a DM on IG if you'd like to see some pics!

Hey mate!
Yeah Nathan Carothers uses that same method as well, it seems to produce good results... The issue is that I absolutely cannot change the radius in my plunge line, milling like you do requires that the radius in the plunge line be the same as the radius on the tool. Which is great if the knife was designed around that consideration, but the Resolute wasn't and changing it would alter the appearance of the knife quite a bit unfortunately.

Otherwise I would absolutely use this method!
 
You've already got some plunge radius there anyways, what's it at roughly now? You could probably get away with a 3/8" dia EM and be fine as well. I posted a video on IG a couple weeks back showing how I draw my primaries and plunges. Makes it super easy to mill them based on this method and it matches how they're done on a belt as well.
 
You've already got some plunge radius there anyways, what's it at roughly now? You could probably get away with a 3/8" dia EM and be fine as well. I posted a video on IG a couple weeks back showing how I draw my primaries and plunges. Makes it super easy to mill them based on this method and it matches how they're done on a belt as well.

Radius in the plunge line is only 0.06" now, biggest I could go without altering the design is 0.125"...

Also in my experience making angled fixtures like what you're having to tackle is much more of a pain than making a fixture that's flat in the XY plane. I'd rather avoid that if at all possible!
 
For the angle I've just been making the main fixture flat and cutting a set of soft jaws with a surfaced face to hold the main fixture on the angle.
 








 
Back
Top