Cutting dovetails, how hard can it be...

[Jinx-)]

I set Bridgeport for some dovetail cutting using 1 3/8" cutter by F.K.D, I was running 100 RPM and feeding 3.0 IPM for plain 1020, I had radius comp on, which initially was 250 thousands more then actual tool radius and conventional milling, anyway after first pass which took .100 I decreased radius comp by .05 and then it happened, my coffee mug felt from work table, it was like the whole table with my part was beating against the cutter, I reduced feed rate almost to 0.5 IPM and only then beating stopped, but it still chatter. So what have I done wrong, I was running HSS tool using optimal speeds and feeds...
Here few images when chatter started:

here I reduced feed rate, but it still chattered

 

[Browninglover1]

Were you really only running at 100 rpm? That seems super slow to me.

 

[Jinx-)]

yes I was... Optimal cutting speed for 1020 is like 35ft/min RPM's should be even less like 97. Also I was using .0022 chip load and that thing got 10 teeth...

 

[xbowhntr]

I use tooling like this on an old Brigport , your cutter looks like one is tooth is chipped .

 

[Trickymissfit]

I set Bridgeport for some dovetail cutting using 1 3/8" cutter by F.K.D, I was running 100 RPM and feeding 3.0 IPM for plain 1020, I had radius comp on, which initially was 250 thousands more then actual tool radius and conventional milling, anyway after first pass which took .100 I decreased radius comp by .05 and then it happened, my coffee mug felt from work table, it was like the whole table with my part was beating against the cutter, I reduced feed rate almost to 0.5 IPM and only then beating stopped, but it still chatter. So what have I done wrong, I was running HSS tool using optimal speeds and feeds...
Here few images when chatter started:

here I reduced feed rate, but it still chattered

1020 CRS dosn't cut well with a lot of contact area. (material is very gummy like in nature) There's a couple ways to get around a lot of this, and really the best way is to use a different cutter. I used to grind the desired dove tail onto end mills (I think you can buy them already ground). You need a good spray mist coolant to keep the temps down and lube the bottom side of that dovetail cutter. But an even better material for your use would be generic 8620 (you can buy it in a ground finish to save some work). Still remember your milling the dovetail, and it will never be that quality of a dove tail cut on a shaper with single point contact, or wiring the shape out. We kept an old G&E shaper in the shop just for cutting precision dove tails as it was far more accurate.

Next time look around for a piece of 8620 bar stock, or even O-1 gauge stock. Make a roug cut with about .0075" stock left on the bottom flat face. Use something like grinder coolant with a little bit of cutting oil added to it (maybe one cup per gallon). There is a way to regrind the dove tail cutter if there's not enough bottom relief, but the end mill already has it and cuts better.
gary

 

[Trickymissfit]

yes I was... Optimal cutting speed for 1020 is like 35ft/min RPM's should be even less like 97. Also I was using .0022 chip load and that thing got 10 teeth...

that's a good cutter. I was thinking you were using one of the old style ones that had little reliefe on the bottom side. Another thing that will really help your dove tail is to relieve the female corner of the dovetail about .06". Most guys don't like to do this as it involves two setups. Make a rough cut leaving about six to eight thoundths stock to be cleaned up. Then cock the head about five degrees and go back into the female corner with a .06" saw cutter about .04" deep. Then realign the head and make a finsh cut. This method really helps cutting the angled part.
gary

 

[Jinx-)]

I think I need to resharpen primaries and secondaries on the bottom and add more relief, just like on endmill where its cutting just on the edges when facemilling so it would have more clearance and not rub and chatter like it does now.

 

[Trickymissfit]

I think I need to resharpen primaries and secondaries on the bottom and add more relief, just like on endmill where its cutting just on the edges when facemilling so it would have more clearance and not rub and chatter like it does now.

That's the one advantage of cutting dovetails with a reworked end mill. Unless I was going to scrape the dovetails (usually cast iron), I always put a small relief in the large flat surface. (not much, and usually under cut by about .003" - .005") The .06" relief in the corner will really help you out in getting the angles to come out right due to the loss of tool pressure in that corner. I did try to cut some dovetails with the ram attachment for a Bridgeport, and trust me they are not good for much of anything in my book. Still nothing cuts dovetails as well as a shaper. I also seriously recommend you trying 8620 hot rolled steel next time. It cuts much better than CRS, and certain lots come with a high sulphur content that will also aid in cutting the stuff. You really didn't do all that bad for cutting CRS
gary

 

[Jinx-)]

Gary, thank you for your advice! After all I decided not to to scrap work I started. I also found interesting article by Peter P. Jenkins president of Harvey Tool Co. LLC, "Dodging dovetailing headaches" Dodging dovetailing headaches | MICROmanufacturing

Well, that article is more about microdovetailing , but it gives very good points what to avoid in dovetail cutting and one of them number 5. Failure to climb mill. So I switched from conventional to climb and here are the results.

Now, if I have to cut my next dovetail, I think I'll get indexable insert cutter and take advantages of higher cutting speeds and feeds

 

[Trickymissfit]

Gary, thank you for your advice! After all I decided not to to scrap work I started. I also found interesting article by Peter P. Jenkins president of Harvey Tool Co. LLC, "Dodging dovetailing headaches" Dodging dovetailing headaches | MICROmanufacturing

Well, that article is more about microdovetailing , but it gives very good points what to avoid in dovetail cutting and one of them number 5. Failure to climb mill. So I switched from conventional to climb and here are the results.

Now, if I have to cut my next dovetail, I think I'll get indexable insert cutter and take advantages of higher cutting speeds and feeds

I thought about the cutter path direction, and sorta figred you were. Just remember to have everything locked down, but the slide. And also tighten the gibs as tight as you can get by with (always adjust them at the far ends of travel, and never in the middle). If your parts are short enough, turn your vise and cut front to back (or vise versa). Then you can lock down the table as thats the first thing that will move on you. Just remember that climb cutting on a finish pass is a one time thing!!

After the other post I remembered why I hated to work with dovetails cut on a mill! They have some much induced stress in them from the end mill that they change all over the place when you scrape them! You don't get that off a shaper using single point tooling. Of course I was working with dovetails that often were an inch and a half tall, but have done some that were only about a quarter inch.
gary

 

[Jinx-)]

I think I dislike working on the Bridgeport mill, even when it does have 30+ year old cnc controller for XY axis, basically it took 8 hours today to contour and cut dovetails and they have -.002 plus nothing tolerance, well its going to be aloris piston tool post when its done, it should resemble something like this http://www.contractmachining.us/forsale/fixed/oct08/dwk12_4968.jpg

 

[Bullet bumper]

You seem to be cutting the base as well as the angle . Dovetail cutters don't like cutting on both faces at the same time The shoulder for the dovetail can be cut with a normal end mill but about .015 too shallow. Then use the dovetail cutter so it is only cutting on the side and move in while not cutting anything on the base of the cut . Use conventional milling only and very light cuts. Don't heat up 1020 as it will harden.
When the dovetail is getting near to specks drop it down and mill out the .015 on the base them move in and mill the inner edge to specs.
From the chips on the edges of the cutter you are just going in too deep at a time . They are very slow cutting and you have to be patient .

 

[Jinx-)]

That's what I did, I used 3/4 endmill to form a frame, it took 650 thousands on both sides and 400 thousands deep, then I switched to dovetail cutter and did five more frames while compensating for diameter of the cutter on every pass, plus when cutting frame it has final pass option which I set to 0.005.

 

[Jinx-)]

About climb milling, here is what I found about dovetail cutting from that article I listed before.

5. Failure to climb mill. Although conventional milling has the benefit of gradually loading the tool, in low-chip-load applications (as dictated by a dovetail cutter's small neck diameter) the tool has a tendency to rub or push the workpiece as it enters the cut, creating chatter, deflection and premature cutting edge failure. The dovetail has a long cutting surface and tooth pressure becomes increasingly critical with each pass. Due to the low chip loads encountered in micromachining, this approach is even more critical to avoid rubbing. Although climb milling loads the tool faster than conventional milling, it allows the tool to cut more freely, providing less deflection, finer finish and longer cutting-edge life. As a result, climb milling is recommended when dovetailing.