| Gallery, Projects and General > How do I?? |
| Milling Dovetails |
| (1/3) > >> |
| Chuck in E. TN:
I am in the middle of making Harold Halls Deluxe Grinding Table. I need to mill dovetails in several parts. The dovetails are 60° and 8 mm (.314 in) to 8.5 mm (.335 in) high, length up to 50 mm. As Im getting ready to order my first dovetail cutter, what size is recommended? I will be ordering the cutter from LMS and sizes available are 3/8, ½ and Ύ in. The cost difference isnt that much, but I dont want to order all three now. Any other comments on milling dovetails welcome, as Ive not done them before. Speeds and feeds? DOC? Multiple passes? Material is mild steel. Mill is an HF X2. Go easy on this noob, eh? Thanks in advance. Chuck in E. TN |
| Lew_Merrick_PE:
Chuck, Get the largest diameter that will clear your dovetail. I am not sure what an "HF X2" mill is, but I assume it is some type of mini-mill. Clear as much material out of the way as you can with regular end mills before using your dovetail cutter. If at all possible, get two cutters. Identify one for roughing out the dovetails and keep the second as a finishing cutter that will stay sharper longer because of the limited number of lighter cuts. I don't think I have ever successfully taken a dovetail cut more than (about) 1/8 inch of material removal -- and that was on a rigid column mill, not a light mill. I usually limit such cuts on my "mill/drill" (that started out life in 1976 as a JET-16 unit before it was dropped off a loading dock) to about .050 inch when roughing. Finishing cuts are usually in the less than .015 range. The recommended cutting speed for LC steel (1015-1020 assumed) is 80-150 surface feet per minute. As I am assuming that you are running a light mill with lots of flex (as compared to, say, a Gorton 9J vertical mill), run towards the bottom end of the speed range and subtract (about) 20%. 80 SFM is 960 surface inches per minute. Divided by pi gives you 305.6. Divide that by the largest diameter (in inches) of you cutter to get your RPM. You should be able to use as high a feedrate as your mill will handle without vibrating the cutter too badly. Were this being done on a truly rigid mill, I would set the cutter speed at about .008/flute (i.e. .008/flute * Number_of_Flutes * RMP = inches per minute feedrate). Does that help? |
| DaveH:
Chuck, See if I can add a little, to what Lew as said. With respect to Lew, forget the manufactures data regards feeds and speeds they are not for you and me with home workshop type mills. Semi and industrial machines fine. Make sure the work piece is held in a rigid manner. Only cut one side of the dove tail at a time. Use the largest cutter possible. Only cut in conventional milling. (Not climb milling) :hammer: Make sure the two unused axis are locked. Take it slow and steady. First cut the slot out with a normal end/slot mill. Now for the dove tail. Start with a spindle speed 500/700 rmp first cut tiny .005, a slow and steady speed careful when the cut first starts making sure it is just cutting not too fast listen and feel the machine. At the end of the cut, remove all chips then return the cutter to the start. Two ways here either leave it running, or stop the spindle and return, if you stop the spindle you can then turn the cutter by hand so it does not touch the work piece. It is not a good idea to cut on the way back. :hammer: Now remember each time the cutter it set into the work piece the load on the cutter increases, there is more cutter surface in contact with the work piece. So as you cut more of the dove tail you may have to reduce your feed. Try to keep clearing the chips away. If you are happy and the machine was happy you could in crease the speed, and feed rate, keeping the same .005 cut. Everything good no bad vibrations increase the cut say to .010 or even .025. Listen and feel the machine, it will start to complain, take notice or your cutter may break. Finish cuts of .002 or even .001 if you have to are OK, just increase the feed a little. Chuck, it is a bit of a slow process, take your time, feed especially slow when the cutter just starts to cut, then speed up. Try to keep the chips away. I hope this helps a little, its one of these things that is much easier to show than explain. :beer: DaveH |
| Jonny:
--- Quote from: Chuck in E. TN on July 07, 2011, 10:54:53 AM ---The dovetails are 60° and 8 mm (.314 in) to 8.5 mm (.335 in) high, length up to 50 mm. 3/8, ½ and Ύ in. --- End quote --- Just measured a 3/8" as best i can, the max depth you will achieve is 4.5mm. An 1/2" decent quality one i have here can only achieve 4mm depth! All the same a 3/4" on an X2 will be asking for trouble, underpowered and serious flex. Soon find out when cutter lasts a couple of minutes. Sound advice from Dave i always ignore recommended speeds and 'get a feel for it', dont force it. You can get a far better finish by climb milling, i do it all the time especially on precision dovetails. Plenty of coolant as well. |
| DaveH:
Jonny, --- Quote from: Jonny on July 07, 2011, 04:52:34 PM ---You can get a far better finish by climb milling, i do it all the time especially on precision dovetails. Plenty of coolant as well. --- End quote --- Ah... but do you climb mill on a X2, and if he doesn't have flood coolant? DaveH |
| Navigation |
| Message Index |
| Next page |