Re: [CAD_CAM_EDM_DRO] Digest Number 505
Posted by
Fred Smith
on 2000-05-25 07:36:06 UTC
Tim,
I usually recommend that people touch off the face of the part, rather than the chuck or some other place. This makes all your Z's that are cutting material a negative number, and is usually a "Safer" approach to CNC turning. It's also easier for me to read & understand the code ;-)
Vector Lathe roughing function can generate the roughing passes in either a horizontal or vertical direction. It also generates a finish pass, comped for the tool radius. If you are using a sharp HSS turning too, that will not be much of an issue, but if you decide to grind a radius on the tool nose (to improve surface finish with higher feed rates), or use indexable carbide insert tools it becomes a concern. The simple method from a manual programming standpoint is to add the tool radius to the desired finish radius for external and subtract it from internal corners. For the 3/4 diameter aluminum rod, the finish pass would be the radius plus the Tool nose radius .375 + .03125 (1/32 tnr) = .406 R Because the geometry is so simple, it may be easiest to just program a cut from
G01 X-.0620 Z0.4060
G03 X.7500 Z0.0000 I0.0 J-.4060
And repeat it every .02 in a minus Z.
However, because most lathes will exert more force, with improved cutting capabilities when pushing the tool in toward the chuck, rather than pushing perpendicular to the spindle axis, I would try to cut this by using the horizontal roughing passes. The depth of cut can probably be increased to .040-.050 (maybe more) if cutting in this manner, rather than trying to cut the full radius for each pass, and it will also eliminate the air cuts.
Listserve Special discounts and offers are at: http://209.69.202.197/cadcamedmdro.html
imserv@... Voice:248-486-3600 or 800-386-1670 Fax: 248-486-3698
I usually recommend that people touch off the face of the part, rather than the chuck or some other place. This makes all your Z's that are cutting material a negative number, and is usually a "Safer" approach to CNC turning. It's also easier for me to read & understand the code ;-)
Vector Lathe roughing function can generate the roughing passes in either a horizontal or vertical direction. It also generates a finish pass, comped for the tool radius. If you are using a sharp HSS turning too, that will not be much of an issue, but if you decide to grind a radius on the tool nose (to improve surface finish with higher feed rates), or use indexable carbide insert tools it becomes a concern. The simple method from a manual programming standpoint is to add the tool radius to the desired finish radius for external and subtract it from internal corners. For the 3/4 diameter aluminum rod, the finish pass would be the radius plus the Tool nose radius .375 + .03125 (1/32 tnr) = .406 R Because the geometry is so simple, it may be easiest to just program a cut from
G01 X-.0620 Z0.4060
G03 X.7500 Z0.0000 I0.0 J-.4060
And repeat it every .02 in a minus Z.
However, because most lathes will exert more force, with improved cutting capabilities when pushing the tool in toward the chuck, rather than pushing perpendicular to the spindle axis, I would try to cut this by using the horizontal roughing passes. The depth of cut can probably be increased to .040-.050 (maybe more) if cutting in this manner, rather than trying to cut the full radius for each pass, and it will also eliminate the air cuts.
> Date: Wed, 24 May 2000 09:35:14 -0600Best Regards, Fred Smith- IMService
> From: Tim Goldstein <timg@...>
>Subject: RE: Newbie - G COde question
>
>I just had Vector spit this out for me. It is setup for a traditional lathe
>layout with Z axis being the length of the bed and X axis controlling the
>diameter of the part. It is setup as follows:
>Z0 Z0.625
>_________)
>
Listserve Special discounts and offers are at: http://209.69.202.197/cadcamedmdro.html
imserv@... Voice:248-486-3600 or 800-386-1670 Fax: 248-486-3698