Question about using a dovetail cutter

Hi,

Simple question, really. I have a new tool on the way for cutting 5th axis dovetails. I was wondering if this tool (I don't have it in my possession yet) would also be suitable for taking a light face cut to flatten my part. This would save a tool change and speed up my process. Looking to take a max of about .020, just to flatten the top.

303 Stainless
2013 Haas VF4SS
Flood Coolant
Part is 1 x 1.5 x 1.75

For 303 the website shows 300-600 SFM and .003 to .006 IPT. WOC says .120 and DOC says application dependent. Should I be able to take this in 2 passes per side of dovetail coming in from the side?

Thanks for your help,
Alex

I does not look like your pictured cutter would be happy.
To face mill the center and the insert ass mounted end needs to be inside the tips and the picture does not look like this is so.
If the tips "proud" then yes it will cut but still don't think it a good idea if you have room in the toolchanger for a facemill.
Bob

I don't think so either. The tips of dovetail cutters are sort-of delicate. Generally I only cut as little as possible with it. I suggest starting with an endmill and flattening the whole bottom and step it out to the dovetail with the endmill then cut the dovetail with the dovetail cutter.

You don't spend the extra money for an SS machine to get so cheap on the tool changes that you would do something as hinky as this.

You already have a tool in the spindle for roughing the "shoulders" of the dovetail, right? So just use that to clean up the top of the dovetail. Maybe pick a diameter wide enough to face the top of the dovetail in one pass, as well as rough the shoulders. The finish on the top of the dovetail isn't critical since that's not a reference surface.

No doubt you could do it with the dovetail cutter, after all, it's capable of undercutting the dovetail. But, I don't thank its a first choice for a face mill, or a rougher for stainless.

For aluminum, we undercut/finsh the dovetail in two passes with that tool, easily. Haven't tried it with stainless.

Hi crane550:
A couple of things:
First your dovetail as drawn in your picture show a sharp internal corner.
Is this really what you hope to make, and does your cutter really have the dead sharp points necessary to mill this shape?
If so, the cutter will be fragile and will not make many parts even in 303 SS before the points are gone.
It will also not face worth a shit if the points are sharp or close to it.

Second, how deep is the dovetail?
I've found that just plowing it into the side of the job at full depth makes both a shitty job and beats the cutter and the machine spindle to ratshit if the dovetail has any depth at all.
A 0.050" deep dovetail is probably fine, even a 0.100 deep dovetail is probably fine but a 0.200 deep dovetail, especially an acute angle dovetail is hard on the cutter and often will wipe out the points in stainless steel, even babying the feedrate.

So I take the extra time and walk down down the sidewalls in successive passes in order to preserve the cutter.
This of course violates the rule of going balls out fast, but it's cheaper on inserts and it keeps the noise level down and makes a better dovetail too.
The pointier the points on the cutter, the less I want to load them.

But you're talking about making time on these, so you will have to accept a shittier dovetail cut in one go as a result and you'll have to change out your inserts more.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Not only would I use a small facemill I would also use it or an endmill to bulk out all the material that doesn't need a dovetail cutter to be removed

Insert not included as per add so likey you need to indicate the 45* to very close. Not a whole lot you can do except to see the inserts run very true.

You might check the end to see clearance and dish and with that and with the ends running .0005 all the same you might use it to flatter the top..

*But much better IMHO to use an end or a face mill
https://www.tecus.com.tr/wp-content/uploads/2018/07/DC1750-45.pdf

Hi michiganbuck:
You wrote:
You might check the end to see clearance and dish and with that and with the end running .0005 all the same you might use it to flatter the top..
If an insert tip is protruding further than its mates the cutter will act like a flycutter and will lose the tip of that insert early.
It will also leave a crappier surface finish, but it will not fundamentally keep the cutter from doing its job.
This is because the feedrate chosen assumes all the cutting load will be shared by all the inserts so if only one is cutting there will be swirl marks in the finish.

However as you correctly point out too, if the heel of the insert is hanging down, you will not get a flat surface.
An insert tip hanging down is not that uncommon, but an insert heeling down would mean the cutter manufacturer fucked up the positioning of an insert pocket which I must believe is very rare.

Of greater concern, in my opinion, is whether the tips of the insert have a big enough radius to handle the DOC.
A very small tip rad and a DOC that is bigger than that rad will encourage the inserts to act almost like a plow...pushing up a big bur and making the insert want to dive downward into the surface.
Even though the spindle bearings can handle it unless they're totally hooped, the finish is typically terrible as the cutter is forced downward into the finished surface.

So I concur that unless the tip rad is bigger than 0.020", a cut of that depth will be rougher than a badger's ass.
It's just a holding dovetail so maybe the OP doesn't need to care, but if he has to change fucked up inserts all the time he'll care soon enough.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

implmex said:

Hi michiganbuck:
You wrote:
You might check the end to see clearance and dish and with that and with the end running .0005 all the same you might use it to flatter the top..
If an insert tip is protruding further than its mates the cutter will act like a flycutter and will lose the tip of that insert early.
It will also leave a crappier surface finish, but it will not fundamentally keep the cutter from doing its job.
This is because the feedrate chosen assumes all the cutting load will be shared by all the inserts so if only one is cutting there will be swirl marks in the finish.

However as you correctly point out too, if the heel of the insert is hanging down, you will not get a flat surface.
An insert tip hanging down is not that uncommon, but an insert heeling down would mean the cutter manufacturer fucked up the positioning of an insert pocket which I must believe is very rare.

Of greater concern, in my opinion, is whether the tips of the insert have a big enough radius to handle the DOC.
A very small tip rad and a DOC that is bigger than that rad will encourage the inserts to act almost like a plow...pushing up a big bur and making the insert want to dive downward into the surface.
Even though the spindle bearings can handle it unless they're totally hooped, the finish is typically terrible as the cutter is forced downward into the finished surface.

So I concur that unless the tip rad is bigger than 0.020", a cut of that depth will be rougher than a badger's ass.
It's just a holding dovetail so maybe the OP doesn't need to care, but if he has to change fucked up inserts all the time he'll care soon enough.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Click to expand...

Agree it could be like a fly cutter if it has proper clearance to the end and OD, and has some dish..

Wow, thanks everyone for the feedback! Seems like the general consensus is no, don't try it.

Tool changes are quick, so it's really not a big deal. It's just a super quick operation and I was hoping to kill two birds with one stone. I have a 2" face mill with 90 degree side cutting capabilities, which should work nicely for skimming the top.

The inside corner doesn't have to be perfectly square, and the dovetail cutter does indeed have a radius. This was taken into account with the design. Will try to post a video when it's up and going.

Alex

looks like the radius is .014 and the body is dead flat to the inset. So likely there would be little chance of using the end for cutting the part top. Even if .010 hang out that would not be enough for chips clearing enough to not be a problem.

Re:https://www.tecus.com.tr/wp-content/uploads/2018/07/DC1750-45.pdf

crane550 said:

Wow, thanks everyone for the feedback! Seems like the general consensus is no, don't try it.

Tool changes are quick, so it's really not a big deal. It's just a super quick operation and I was hoping to kill two birds with one stone. I have a 2" face mill with 90 degree side cutting capabilities, which should work nicely for skimming the top.

The inside corner doesn't have to be perfectly square, and the dovetail cutter does indeed have a radius. This was taken into account with the design. Will try to post a video when it's up and going.

Alex

Click to expand...

definate no on it being a face cutter, the picture makes it look like the dovetail sits recessed from the end of it.

I would like to add that if you were cutting 6061 aluminum, you would probably get away with it.

303 is like the 12L of stainless, and I still would not do it.

Hi Folks,

Just wanted to report back. I got myself a 7 flute 2" face mill, and am using that for my initial face. To be honest I was hoping for better surface finish. I went with a 90 degree face mill since I need to do shoulder work as well. Seems to work OK but I think my surface finish leaves a bit to be desired. I was hoping to get away with using this to mill the exposed surface in a later op.

Here is a video:

Shared album - Alex Crane - Google Photos

Here is what I am running:

303 Stainless

Face Mill:
2" 90 Degree
500 SFM (954 RPM)
.007 Feed per Tooth (47 IPM)
.020 Faceing Pass, then .180 wide by .08 deep shoulder

Dovetail cutter:
1.71" 5th Axis
550 SFM (1173 RPM)
.004 Feed Per Tooth (23.5 IPM)

Key Slot:
4 Flute .25" EM, 1/2 Stickout
250 SFM (3820 RPM)
.0012 IPT (18.3 IPM)
.08 deep x .250 wide slot cut.

Any suggestions on where to go from here? I have milled a lot of aluminum, and if I was working with that I wouldn't be here. In stainless I'm out of my comfort zone.

Thanks as always, this forum has been a lot of help.

Regards,
Alex

Unfortunately I don't have an example of what you are doing in stainless but the 5th axis dovetail cutter should allow you to do a skim cut across the top. We do that with that exact cutter on aluminum just to make sure that dovetail depth is always consistent. In aluminum it leaves decent finish, 0.006ipt, 3200RPM. I think if you take it down to stainless speed it should work for clean up. In picture, the dovetail step surfaces and top surface are machined with that cutter. I leave about 0.003" for dovetail to clean up at those two surfaces.

For stainless parts facing we use Ingersoll SNGU1205ENN IN2505 inserts in DN6H-25R01 holder. This insert has a wiper and we get mirror like surfaces in 304/316. They have aluminum insert for that same body and we use it for all aluminum facing.

Alex O

Hi crane550:
How come you've got your cutters hanging out so far?
Is there a way you can run shorter toolholders to get the business end closer to the front spindle bearing.
That third cutter in particular sounds like shit.

The facing cutter sounds to me like it's running too fast as well and the big bur you're pushing tells me the inserts are getting to be in rough shape.
303 stainless is the aluminum of stainless steels...you should be able to do far better than what I'm seeing and hearing.

Try dropping your surface speed on the facemill, going with the shortest gauge length toolholders you can get your mitts on and check the inserts to see if they're trashed.

Retire that poor endmill you've been beating the shit out of on the keyways, and consider using the new one to mill those shoulders as well, saving the face mill for facing.
If you are receptive to the idea of high speed milling, you can also try full depth cuts with small radial engagement and high chipload to mill the shoulders.
You can also ramp the cutter into the keyslot with shallow DOC and a high speed ramp so the cutter only ever sees 0.010" or so of material during each pass.
I'll bet you'll get a better looking keyslot just as fast and the cutter will last longer too, especially if you crank up the RPM of that 1/4" cutter.

Stainless steel loves to push a big bur when you get too aggressive with MRR...even though 303 is the aluminum of stainless steels it's still not quite like aluminum and needs a different touch.
I've always done much better with fast light passes than I've ever done with big hogging cuts in stainless steels of all kinds

But do something about that long toolholder stickout first and I'll bet all your problems will go away like magic.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Hi Marcus,

I need the length for a different operation when it's on the rotary table. Same with all the cutters- they are as short as I can given the situation.

That shell mill and inserts are brand spanking new. That video was literally the 2nd cut it's ever made. This is brand new to me. The end mill is fairly new as well. I did some other operations with that same 1/4" EM on the same 303 block (I continued to try the next operation) and it performed beautifully. Sounded good and left a good finish.

I completely agree that shorter is always better, but my setup has some limitations with my rotary. I could set up 2 end mills, but I hate doing that if I already have something in the machine that will work. I'm perfectly fine going super light on this OP to save an extra tool slot.

I think your idea on the ramping is a good one. I will try it. I will also lower my SFM for the face mill and see what happens. Honestly I didn't know if I should go faster or slower, so thanks for the tip.

On 2nd thought, the dovetail cutter can certainly be shorter, the hard holder is just what I happened to have free at the moment. But that cutter seems to be working fine, and it even seemed to like a slight increase in SFM.

Hard to have much more fun than this on a Friday night! Up until now every product we have made and sold has been aluminum. Time to get out of my comfort zone. Hopefully in a few months 303 will feel as unintimidating as aluminum is.

Re Implemx [How come you've got your cutters hanging out so far?]
long hang out can cause dulling and a less good finish.

More teeth in the cut may help finish.

*Nice looking finish part.

Limit SFM to 300 when cutting steel/stainless with coolant to avoid thermal shock.

0.007 IPT on a 90-degree facemill will not leave you a good finish. Try 0.003.

No way around hitting those burrs with a chamfer mill.