Re: holey pear was4th axis rotary (and other tricks)
Posted by
ballendo@y...
on 2000-09-05 16:03:06 UTC
Alan, and Bill, and Darrel,
Just saw your post of the part, Yep, it's what I thought except the
slot 'tween the ears follows the path of the bore. I know it looks
better that way, but does it hafta? If so, it's lathe or trick time.
Lathe is obvious, trick is:
1. clamp a thick sub-plate on the mill table, hangin' over the front
of the table (he has a sherline,guys)
2. mill the overhang to a clean 90. We'll use it later.
3. clamp the stock (1.125x1.875x.750 (or so))with straps that clear
the bore and part outline locations.
3a. (added on re-read,forgot the thickness) mill the area of the part
to thickness (could use a pocket routine here,so you dont hit the
clamps holding the stock edges.
4. Do the bores. (drill 1st will take the end load off the endmill)Or
use all this helical stuff we been talkin' 'bout. :)
Be sure the big bore goes into the sub base a ways.(trick is coming)
5. tap the drill holes darrell mentioned (in the sub base) and use w/
bolts to hold the part for the outline milling.
6. Do the outline.
<aside>
Bill, Using different than actual offsets with G41,G42 is common.
Darrel mentioned how in the previous post. If the offsets bigger than
the tool really is, we cut bigger parts.(roughing passes)Change the
offset to match reality and we cut finish size. Offsets are also
adjusted to deal with sharpened or just plain wrong-sized cutters.
A lot of shops program tool centerline(at the arbitrary tool value)
and adjust the offset(nominally 1/2 tool dia.) to match the REAL
world.
Alan, any reasonably current MaxNC DOES have G41,G42. Practice "air
cutting" before you rely on it, tho. Also, the blue insulation board
sold at Home Depot works well for this type of "proofing" parts while
learning. Dust is not TOO bad. Thanks to RON at Flashcut for this.
</aside end>
7. Now,part is done, except the "ears". Remove the sub-base and re-
mount with an angle block so the "holey pear" is in the natural
position(upright)Use a piece of stock the size of the big bore to
locate and "pivot" the part. Run a boltand heavy washer(s) through
the middle of this locating pin to hold the part while you machine
the slot(end mill or slit saw) Rotate the part, re-clamp, and re-cut
until you have that "he musta made this on the lathe" look.
Hope you read through before you began. You can see the sub-base
layout needs some pre-thinking.
Ballendo (with thanks to darrel and bill)
P.S for the list:
NO, I'm not going to turn this into a metalworking how-to site(and
clog your emails (I read online) with stuff you already know. This
seemed to be a worthwhile tip to share (others can use, and we've got
some new people) Back to Cad/cam/edm/dro!
Bill wrote:
I read somewhere that by changing the tool diameter that you would
creep up
on the final outline, but I don't know enough to say how it works,
maybe some
others will elaborate. I think it is when the software CNC sets up
the
offset, for a given tool diameter, and thus whit a tool diameter
entered it
will cut at different offsets from the desired outline. I could also
be
completely wrong.
bill
Just saw your post of the part, Yep, it's what I thought except the
slot 'tween the ears follows the path of the bore. I know it looks
better that way, but does it hafta? If so, it's lathe or trick time.
Lathe is obvious, trick is:
1. clamp a thick sub-plate on the mill table, hangin' over the front
of the table (he has a sherline,guys)
2. mill the overhang to a clean 90. We'll use it later.
3. clamp the stock (1.125x1.875x.750 (or so))with straps that clear
the bore and part outline locations.
3a. (added on re-read,forgot the thickness) mill the area of the part
to thickness (could use a pocket routine here,so you dont hit the
clamps holding the stock edges.
4. Do the bores. (drill 1st will take the end load off the endmill)Or
use all this helical stuff we been talkin' 'bout. :)
Be sure the big bore goes into the sub base a ways.(trick is coming)
5. tap the drill holes darrell mentioned (in the sub base) and use w/
bolts to hold the part for the outline milling.
6. Do the outline.
<aside>
Bill, Using different than actual offsets with G41,G42 is common.
Darrel mentioned how in the previous post. If the offsets bigger than
the tool really is, we cut bigger parts.(roughing passes)Change the
offset to match reality and we cut finish size. Offsets are also
adjusted to deal with sharpened or just plain wrong-sized cutters.
A lot of shops program tool centerline(at the arbitrary tool value)
and adjust the offset(nominally 1/2 tool dia.) to match the REAL
world.
Alan, any reasonably current MaxNC DOES have G41,G42. Practice "air
cutting" before you rely on it, tho. Also, the blue insulation board
sold at Home Depot works well for this type of "proofing" parts while
learning. Dust is not TOO bad. Thanks to RON at Flashcut for this.
</aside end>
7. Now,part is done, except the "ears". Remove the sub-base and re-
mount with an angle block so the "holey pear" is in the natural
position(upright)Use a piece of stock the size of the big bore to
locate and "pivot" the part. Run a boltand heavy washer(s) through
the middle of this locating pin to hold the part while you machine
the slot(end mill or slit saw) Rotate the part, re-clamp, and re-cut
until you have that "he musta made this on the lathe" look.
Hope you read through before you began. You can see the sub-base
layout needs some pre-thinking.
Ballendo (with thanks to darrel and bill)
P.S for the list:
NO, I'm not going to turn this into a metalworking how-to site(and
clog your emails (I read online) with stuff you already know. This
seemed to be a worthwhile tip to share (others can use, and we've got
some new people) Back to Cad/cam/edm/dro!
Bill wrote:
I read somewhere that by changing the tool diameter that you would
creep up
on the final outline, but I don't know enough to say how it works,
maybe some
others will elaborate. I think it is when the software CNC sets up
the
offset, for a given tool diameter, and thus whit a tool diameter
entered it
will cut at different offsets from the desired outline. I could also
be
completely wrong.
bill