Printable View
Hi,
I have to make thin brass washers.
ID=9.5 mm, OD=16mm. Thicknes= 0.3 ; 0.5 ; 1 and 2mm
(ID=0.374'', OD=0.629''. Thicknes= 0.0118'' ; 0.0196''; 0.0393'' and 0.078'')
Is there some special trick to create a burr-less part?
What cutting speed and feed do you recommend?
Im using this cut off tool:
Iscar Catalog : PENTA 24N-J - 6003226
IC908
Here is a photo of my washers with burr:
ImageShack® - Online Photo and Video Hosting
Radius or chamfer the corners.
The burr is there because the nose of your tool is square. It needs to be angled to minimize the burr.Quote:
......Is there some special trick to create a burr-less part?.....
Gene
One way to almost elimiate that burr is to use a threading tool to make a small vee groove on the inside, inline with the corner of the parting tool then the part breaks off almost clean. (see the picture) The smaller the nose radius on the threading tool the cleaner the part off.
Thank you for your answers.
I don't have tool for inside groove. Any other idea ?
Why would this help ? I will try this.Quote:
Originally Posted by txcncman
Okay, just bore you ID deep enough to meet the leading edge of the parting tool and your part will come off with a minimal burr.
Make one.Quote:
Originally Posted by haklc
Use a regular HSS boring bar, and just grind the relief back to a 45deg angle.
I'd use a T shaped cutoff blade, sharp, with about a 15-20 angle on the front (viewed from the top of the tool), and just keep the tip sharp.
I've run this configuration for decades on automatic screw machines, brass parts, and never had a problem with burrs.
Somma Tool Company - T-Type Cut-Off Blades H.S.S.
Thanks a lot :)
What cutting speeds and feeds are most optimal for boring and cutting off ?
Geof's first post is the ideal way. I use a threading insert such as an NT-1L, NT-2L or NTF-2L or BNVR-60 (or carbide threading bar with a .003R (inch) depending on hole size) to machine a 45 degree chamfer on the ID at the cut-off position. I program it to go .003 (inch) past width of washer. This can be very critical. Too far past and it leaves a burr on the cut-off face. Not far enough and it pushes a burr onto the 45 degree. Angled cut-off insert is not necessary for most materials, and in fact is often detrimental to keeping the faces parallel and maintaining a good finish.
If using an insert, use one with a small radius. The bigger the radius on the insert the harder it is to cut the washer off burr free. In other words don't use a 16 NR 12UN insert to chamfer with...use a 16 NR A60. Of course you don't want a sharp point or the finish will be horrible. Plus it won't hold up very long. We don't run brass washers, but run tens of thousands a year...mostly out of 52100, 440C and 420.
As far as feeds and speeds are concerned in brass, I push feeds as fast as I can and still maintain the needed finish. I run RPM as fast as the machine will allow although I have been limiting the 5000 rpm lathes to 4000 rpm in most cases. Cut off rpm is limited to 3000 rpm, sometimes less. If adjusting Z offset still leaves a burr, I will try slowing the feedrate down for the last .030/.050 (inch) before part drops off. Most times I cut off at F.002 (inch). Too high rpm and part flies. Too fast feedrate and part not only sometimes flies, but comes off with a more pronounced burr.
Occasionally I can't get rid of the burr, but it usually is light enough that tumbling the washers removes the burr. Be aware that even a burr free part will have a sharp edge at the junction of the cut-off face and the chamfer.
I've used the Penta-Cut insert with no problems.
BTW, this method works with other parts as well.