LinkBack URL
About LinkBacks
Thats scary you need a wider parting tool to do it.
Slow down when you drop the part.
I dont peck my parting tools either.
| | |
I was asked to try parting some 6061 aluminum solid round stock, 4" diameter,6" slug. The parting tool is .098 wide. The part will .250 wide. I am concerned about safety, ridgity,tool deflection. Any positive advice would be deeply appreciated.
Eric
Thats scary you need a wider parting tool to do it.
Slow down when you drop the part.
I dont peck my parting tools either.
I agree with the scary part.
I would but a spare window for the machine, You may need it.
Run the last 0.5" very slow something like a few hundred RPM
There's no way you could cut it out of 1/4" plate???
The whole idea behind the geometry on most part off tools is the dip in the insert that causes the chip edges to curl in and become less wide than the groove itself. The problem is that you have to push the feed hard to get the result, and pushing the feed hard for 2 inches is going to generate A LOT of heat IE tool failure. I vote no. Unless you can open the groove up and cool it off.
Robert
The beaten path, is exclusively for beaten men.
Try it on a manual lathe first then you will appreciate the problem.
Slow, solid feed, lots of coolant, or better still cutting oil.
Max speed 350. A very tall (2") strong tool will work if the material is OK.
Don't expect a straight cut once the tool loses its edge, which must be perfect.
If it is crappy al. the give up.
Like the man from Krypton says, cut it out of plate.
Super X3. 3600rpm. Sheridan 6"x24" Lathe + more. Three ways to fix things: The right way, the other way, and maybe your way, which is possibly a faster wrong way.
I would use at least a 3mm (.125") wide insert and blade or even 4mm. I know it wastes quite a lot of material on a job like this, but its been my experience that 1/8" inserts and blades will survive reasonably well if you've got good coolant flow. A narrower kerf is difficult to get the coolant into. 2" radial depth is about the maximum I would attempt with the 1.25" blade.
Straightness on the partoff face can never be guaranteed, and a secondary facing operation should be planned for, if for no other reason than to remove chip scuffing or a retraction spiral groove.
I would use CSS at 800 sfm, .004"/rev feedrate, and not stop until I get to X0.25, then slow the feed to .002 and move to X0.125 then retract the tool, stop the spindle. Throw a rag over the piece and grab it and twist it off. You might have to fine tune this a little bit, so that the part does not drop off at the end of the parting cycle.
Don't forget to clamp the spindle speed because you're going to hit the max rpm fairly quickly. Because I use a fairly heavy duty lathe with a 12" chuck, I tend to chicken out at 1500rpmI like to keep the cutting speed reasonably fast for aluminum because the chip comes off smoother. Slowing down is counterproductive, and typically you start getting jam ups when you do this.
Peck parting does not work IMO, because it can be problematic to get the chipflow reestablished in mid cut. You want enough feed rate to make clockspring chips or this whole procedure is going to be a nightmare.
If it so happens that the part has a hole in the center, I have on occassion, rigged up a wooden dowel held in the tailstock, and slide it forward so the dowel is in the hole. Complete seperation is then possible and the part will ride the dowel when it drops off. If something goes wrong, the dowel may get broken, that's why I use wood and not a steel rod.
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Thanks for all the input I truly appreciate it.
Hum, throwing spinning knives at your face. if you going to try it, make sure your turret is straight. And this is where high pressure coolant through the tool really helps. Follow everyones advise on this one.
I believe that Iscar has a through the tool coolant blade that will work well for your situation. It its a DO-Grip Jet Cut good for up to 6.3" diameters according to the book. Looks like you could use a 1.26" blade with a .157" insert and cut off a 4.72" workpiece. Part# DGFH 32-5 Page B119 in my catalog. You will probably need a blade holder too.
No I don't work for them, but they are my favorite for grooving...
Feel free to send me commission Iscar!
Hope this helps,
There are a couple companies that make them. Iscar grooving is my favorite as well.
Posting Permissions
| | |
