Dovetai milling

[wojtek90]

Hi

I have to make 60 degree dovetail in 4140 steel. I have 60 degree HSS dovetail cutter. What toolpath should I use ? depth of cut or approach distant. Should I rough dovetali with another cutter using flowlaine toolpath? I already mill slot.

Any help appreciated.

3-480-052-002.x_t

[htm01]

i would get a carbide or carbide tipped cutter

[nickbe10]

16 hours ago, wojtek90 said:

What toolpath should I use ?

Contour.

Other than that it really depends on what the dovetail is used for.

[crazy^millman]

No faster than about 32 sfm on that tool. Should be able to take one pass and then a spring pass. I use to bury these tools 30 years ago in 4140 on an old Hydroltel at about 1 to 2 ipm.

[Guest]

6 minutes ago, 5th Axis CGI said:

No faster than about 32 sfm on that tool. Should be able to take one pass and then a spring pass. I use to bury these tools 30 years ago in 4140 on an old Hydroltel at about 1 to 2 ipm.

That sounds very reasonable, given a reasonably rigid setup, of course if there was vibration those values might still have to shrink.

[crazy^millman]

21 minutes ago, Peter from S.C.C.C. said:

That sounds very reasonable, given a reasonably rigid setup, of course if there was vibration those values might still have to shrink.

No want to run that in a Weldon holder. I never put HSS tools in a Shrink.

[Guest]

2 minutes ago, 5th Axis CGI said:

No want to run that in a Weldon holder. I never put HSS tools in a Shrink.

Sorry my english was bad there, I meant the sfm and ipm might be lower if the setup is not very rigid. In the past we had some tslot hss cutters we had to machine at .1 ipm because the part was a long narrow shaft held by some clamps and a vblock. 

[crazy^millman]

8 minutes ago, Peter from S.C.C.C. said:

Sorry my english was bad there, I meant the sfm and ipm might be lower if the setup is not very rigid. In the past we had some tslot hss cutters we had to machine at .1 ipm because the part was a long narrow shaft held by some clamps and a vblock. 

Okay Shrink = Slow it down. Sorry I misunderstood.

[#Rekd™]

27 minutes ago, 5th Axis CGI said:

No want to run that in a Weldon holder.

+1000 as it will want to pull down with that dovetail shape!

[wojtek90]

4 hours ago, #Rekd™ said:

+1000 as it will want to pull down with that dovetail shape!

What you mean +1000 ? How about toolpath?

[Guest]

5 hours ago, nickbe10 said:

Contour.

^Contour is a good choice.

5 hours ago, 5th Axis CGI said:

No faster than about 32 sfm on that tool...about 1 to 2 ipm

This should work np. ^

 

[wojtek90]

Make it in one shot or with couple approaching distance "multipasses" .

[Guest]

You could do it in one pass, then take a free pass to clean up the extra Material, the second pass could go a bit faster.

[#Rekd™]

1 hour ago, wojtek90 said:

What you mean +1000 ?

If you do not use a Weldon holder (it has a set screw to hold the cutter into place) the cutter can suck out of the collet as the angular shape is creating downward pressure. Your photo of the cutter has a Weldon Shank for this application.

Yes Contour toolpath, multiple passes if you have room and time....it depends on the tolerance and finish etc.

[E. ARVAI]

2D DYNAMIC PEEL MILL with no micro-lift works gravy for any slotting application

[Leon82]

Draw a line in the center and make your first pass with cutter comp set to off then you can do a pass or two with wear.

[SFricke]

Without knowing much about exactly what you're doing, i would throw in a rough slot first just to get some material out of there.