Hi Jason from Tormach. Let's talk fixture design. I have a piece of drill rod that
I need to put a flat on, and cut a little notch on the end. Simple little part to
do, but I have enough of these to run they I don't really want to load them into
a vise one in time. I need to make small batches of parts like twenty and thirty
at a time, in regular intervals, so every couple of months, or so we need to run
those. Since we normally keep a vise installed in the machines all the
time, I wanted the fixture to be able to just drop into a vise, sit on some
parallels, and run from there. This also ended up dictating how many parts I can
make at a time. The largest part I can really fit into any of the vices that I
have around, is about a four by eight inch part. So I just designed everything
around this size. I decided to use the Uni-force clamp from Mitee Bites for this
project since they allow me to clamp two parts at a time, which helps minimize the
cost of the fixture. Now I just have to sit down and look at the part itself and
figure out how do I want to machine this, and what's the most efficient way to
accomplish all the tasks that we need to. This is really a pretty simple part. We
need to put a flat on the top and cut a notch on it on the end of it. For the
flat, all I need to make sure is I have clearance on the sides or on the top of
my part for the end mill to run over the top. With that uni-force clamp that's a real easy
thing to accomplish. So that just kind of worked out on its own. For the notches I
wanted to keep them facing each other. This allowed me to minimize my cycle
times, and just cut it all more efficiently. If I put them on opposing
faces then I'd have to cut two of them, wrap it all the way across the part and
cut the other side. It's just an inefficient setup. So I ended up putting
a boss in the center of the part, which you can see. And we used these as a bump
stop. So when we slide the bar in, we just bump off for this little boss that's in
the center, and then we can tighten the clamps up. And that gives us our
consistent bump stop...gives us access to the part for the notch, and everything's
in close proximity. So we reduce our cycle times. Once I had this all modeled
into everything, I added some clearance pockets here for the notch itself. So I
just added about fifty thousands clearance on the sides on the width, and
the depth of the pocket just for cutter clearance, and then I just added a
datum hole real quick to make setup real quick, and easy on this. From here we just
need to machine it. So here's some cutting footage of it running on a 770M. We
only needed about five tools to make this part. We roughed it out with a 3/8 inch
end mill. This ran with a half inch depth of cut, with a fifty thousand width of cut.
We used a two way adaptive roughing strategy on this, running at 6100 rpm, at
80 inches a minute. This ran real well. The 2-way adapter strategy definitely
worked out nicely with this part. It really helped the efficiency of the
roughing cycle. After roughing, we came and drilled our tap, and datum holes.
These are 8/32 tapped holes. So we used a number 29 drill, and ran it at 4200
RPM, at 9 inches a minute, with a 50,000 peck depth. Next we came to the quarter
inch end mill. We used this for some rest roughing, and finishing passes. First
thing we did was to bore out our datum hole. We pre-drilled it with that number
29 drill. Then we came back and just plunged the end mill, and with a real
light peck, just to put the datum feature in so that we can indicate this in as a
our zero point. We had a small area that the 3/8th's end mill couldn't reach, so we
just did a quick 2d contour pass to remove this. I'm just ramping back and
forth as you can see. And then we finished up the flats, and the walls with
separate tool passes. These all ran at the same speeds which was 10,000 RPM at 50
inches a minute. After this, we added some quick ten thousands chamfers just to
de-burr the part. This tool ran at 10,000 RPM and 60 inches a minute.
The last tool path we had to run was the thread milling for the 8/32 holes.
We ran the thread mill at 10,000 RPM at 30 inches a minute and we did this in two passes.
The second pass was a real light pass, at five thousands of an inch, just to kind of
take a nice light finish pass, and get a good fit on the threads.
It was pretty lucky on this one. I didn't have to do any cutter compensation, or
anything, to get the threads to fit nice. It just worked beautifully right out,
of the right out of the gate for us. Then once we had this all done, once
everything was all cleaned, up we test fit the holes, and we loaded up some
parts in the clamps to make sure that everything looked good. So thanks for
watching. I hope you guys enjoyed the video. For more metalworking tips, tricks,
and stories, check out our other YouTube videos, and please subscribe.