I designed a couple of parts that I now need to get CNC machined
(mill). I have sent many parts out for laser cutting, but this would
be my first to a CNC shop. As with the laser cut projects, I did the
drawings in Alibre Professional, and now I need to familiarize myself
with the next step for CNC work. I have a couple of small shops that
I am going to approach to run the parts for me, and of course I am

going to ask them how they would proceed... but I would like to ask
the group here what the normal way things happen. Please keep in
mind, I plan to purchase some sort of entry level CNC mill in the next
year or so. Something like a Tormach, or if I could find a used
machine, the Sharp 2412 has been suggested to me... anyways, this post
is not meant to generate talk about the actual machines, more the
methods.

One of my major CNC prep questions is HOW ARE THE PARTS HELD. Both of
these parts are to be milled out of rectangular bar stock, and with
these parts, the finished product will not leave much to hold on to...
hence my concern.

I am trying to incorporate mounting points in the product design, to
allow these parts to be fastened to a jig, but it seems this is a two
step process...

I am picturing in my mind's eye how this would progress thru the
steps.

First I would have to give them (or design for them to machine) a jig
(called jig B) that would hold the parts.

The only way I can envision the next step is for the shop to hold the
raw material (in this case a 4" wide x .750 thick aluminum bar stock)
either on a basic jig (called jig A) on the mill table, or in a simple
mill vice, then run a first program to drill the fixturing holes that
I have designed into the part for second step fixturing in JIG B.
They would then have to remove the part from JIG A and install in jig
B, and run the rest of the program. Is this plausable?

My Next concern would be the something that only the shop I choose
will answer 100%, but could I expect to give them the DFX file and
they then can convert it over to talk to their machines?

Then, how does one decide what tooling to use? We are talking about
smaller shops without the budget for the latest/greatest software...
so does something like MACH3 or the other CAM software pick the tool
sizes? Or does the machine programmer look at the print and say... OK,
I'll use a .250 end mill for here, and a .750 for there, etc??

I suppose this leads to another question... is it prudent for the
person drawing the files to try and use radius' thruout the part that
coincides with common sizes of tooling? I mean if I need a radius on
a part, and the shape is not a critical design element, then Pick
something simple like a .250 radius? Is that just good design work..
meaning everyone in the trade already knows to do that?

thanks alot, I appreciate any helpful comments!

On Sun, 10 Jan 2010 21:28:29 -0800 (PST), rbce2003
wrote:


The only way I can envision the next step is for the shop to hold the
raw material (in this case a 4" wide x .750 thick aluminum bar stock)
either on a basic jig (called jig A) on the mill table, or in a simple
mill vice, then run a first program to drill the fixturing holes that
I have designed into the part for second step fixturing in JIG B.
They would then have to remove the part from JIG A and install in jig
B, and run the rest of the program. Is this plausable?

Ask the shop. If they're really interested in the work, they'll talk
to you. I've seen many parts, like what I imagine yours to be,
machined in multiples from a large piece of material. The material is
clamped to the table on top of a sacrificial plate. A small attachment
to the plate is left as the last thing to be cut, releasing the
individual parts and leaving a skeleton as scrap. But talk to the
shop.


My Next concern would be the something that only the shop I choose
will answer 100%, but could I expect to give them the DFX file and
they then can convert it over to talk to their machines?

Most shops will appreciate a dxf. But I always tell them they use the
supplied dxf at their risk -- the print is the controlling document.


Then, how does one decide what tooling to use? We are talking about
smaller shops without the budget for the latest/greatest software...
so does something like MACH3 or the other CAM software pick the tool
sizes? Or does the machine programmer look at the print and say... OK,
I'll use a .250 end mill for here, and a .750 for there, etc??

Other than obvious things like avoiding sharp inside corners,
especially on deep pockets, let the shop worry about it.


I suppose this leads to another question... is it prudent for the
person drawing the files to try and use radius' thruout the part that
coincides with common sizes of tooling? I mean if I need a radius on
a part, and the shape is not a critical design element, then Pick
something simple like a .250 radius? Is that just good design work..
meaning everyone in the trade already knows to do that?

Give plenty of latitude on non-critical radii. For example:
R .25 APPROX
R .312/.188
R 1/4 (if your title block allows an appropriate tolerance on
fractional dims)
R.25 +/- .03

--
Ned Simmons

Ned Simmons wrote:
On Sun, 10 Jan 2010 21:28:29 -0800 (PST), rbce2003
wrote:

The only way I can envision the next step is for the shop to hold the
raw material (in this case a 4" wide x .750 thick aluminum bar stock)
either on a basic jig (called jig A) on the mill table, or in a simple
mill vice, then run a first program to drill the fixturing holes that
I have designed into the part for second step fixturing in JIG B.
They would then have to remove the part from JIG A and install in jig
B, and run the rest of the program. Is this plausable?

Ask the shop. If they're really interested in the work, they'll talk
to you. I've seen many parts, like what I imagine yours to be,
machined in multiples from a large piece of material. The material is
clamped to the table on top of a sacrificial plate. A small attachment
to the plate is left as the last thing to be cut, releasing the
individual parts and leaving a skeleton as scrap. But talk to the
shop.

My Next concern would be the something that only the shop I choose
will answer 100%, but could I expect to give them the DFX file and
they then can convert it over to talk to their machines?

Most shops will appreciate a dxf. But I always tell them they use the
supplied dxf at their risk -- the print is the controlling document.

Then, how does one decide what tooling to use? We are talking about
smaller shops without the budget for the latest/greatest software...
so does something like MACH3 or the other CAM software pick the tool
sizes? Or does the machine programmer look at the print and say... OK,
I'll use a .250 end mill for here, and a .750 for there, etc??

Other than obvious things like avoiding sharp inside corners,
especially on deep pockets, let the shop worry about it.

I suppose this leads to another question... is it prudent for the
person drawing the files to try and use radius' thruout the part that
coincides with common sizes of tooling? I mean if I need a radius on
a part, and the shape is not a critical design element, then Pick
something simple like a .250 radius? Is that just good design work..
meaning everyone in the trade already knows to do that?

Give plenty of latitude on non-critical radii. For example:
R .25 APPROX
R .312/.188
R 1/4 (if your title block allows an appropriate tolerance on
fractional dims)
R.25 +/- .03



I do CNC programming & setup (20 yrs+). Ned's idea of a sacrificial
plate we use very often. We also use a plate, with counterbored tapped
holes in it. A couple of tiedowns to clamp the part, drill through the
part where the counterbored tapped holes are, blow out the holes, put in
bolts, remove tiedowns, and machine the outer profils.

Also, tolerances dictate cost. The looser the tolerance, the lower the
price. Common end mills (lower cost) come in 1/4 inch increments. If
possible, specify I.D. radii in 1/4 inch increments, and tolerance them
+.015 to +.030, and -0.

Surface finish callouts are beneficial to the quoting process. If not
specified, you may get (and pay more for) a smoother finish than you
actually need.

--
Steve Walker
(remove wallet to reply)

On Jan 11, 8:14*pm, Steve Walker wrote:
Ned Simmons wrote:
On Sun, 10 Jan 2010 21:28:29 -0800 (PST), rbce2003
wrote:

The only way I can envision the next step is for the shop to hold the
raw material (in this case a 4" wide x .750 thick aluminum bar stock)
either on a basic jig (called jig A) on the mill table, or in a simple
mill vice, then run a first program to drill the fixturing holes that
I have designed into the part for second step fixturing in JIG B.
They would then have to remove the part from JIG A and install in jig
B, and run the rest of the program. Is this plausable?

Ask the shop. If they're really interested in the work, they'll talk
to you. I've seen many parts, like what I imagine yours to be,
machined in multiples from a large piece of material. The material is
clamped to the table on top of a sacrificial plate. A small attachment
to the plate is left as the last thing to be cut, releasing the
individual parts and leaving a skeleton as scrap. But talk to the
shop.

My Next concern would be the something that only the shop I choose
will answer 100%, but could I expect to give them the DFX file and
they then can convert it over to talk to their machines?

Most shops will appreciate a dxf. But I always tell them they use the
supplied dxf at their risk -- the print is the controlling document.

Then, how does one decide what tooling to use? *We are talking about
smaller shops without the budget for the latest/greatest software...
so does something like MACH3 or the other CAM software pick the tool
sizes? Or does the machine programmer look at the print and say... OK,
I'll use a .250 end mill for here, and a .750 for there, etc??

Other than obvious things like avoiding sharp inside corners,
especially on deep pockets, let the shop worry about it.

I suppose this leads to another question... is it prudent for the
person drawing the files to try and use radius' thruout the part that
coincides with common sizes of tooling? *I mean if I need a radius on
a part, and the shape is not a critical design element, then Pick
something simple like a .250 radius? *Is that just good design work...
meaning everyone in the trade already knows to do that?

Give plenty of latitude on non-critical radii. For example:
R .25 APPROX
R .312/.188
R 1/4 (if your title block allows an appropriate tolerance on
fractional dims)
R.25 +/- .03

I do CNC programming & setup (20 yrs+). Ned's idea of a sacrificial
plate we use very often. We also use a plate, with counterbored tapped
holes in it. A couple of tiedowns to clamp the part, drill through the
part where the counterbored tapped holes are, blow out the holes, put in
bolts, remove tiedowns, and machine the outer profils.

* Also, tolerances dictate cost. The looser the tolerance, the lower the
price. Common end mills (lower cost) come in 1/4 inch increments. If
possible, specify I.D. radii in 1/4 inch increments, and tolerance them
+.015 to +.030, and -0.

Surface finish callouts are beneficial to the quoting process. If not
specified, you may get (and pay more for) a smoother finish than you
actually need.

--
Steve Walker
(remove wallet to reply)

I would recommend specifying inside radii a little bit bigger than a
common fraction.
For example, an inside radius of .140" will cut smoothly with a 1/4"
endmill, but a .125" radius will chatter and work better with a
smaller endmill, which cuts slower. Modern CNC and CAD/CAM systems
create a toolpath to follow any specified radius, but matching the
radius to the endmill is a Bad thing. In the old days with a manual
machine, using the radius of the endmill to generate the inside radius
was the easiest way to go. Now that is not true.

Also, tolerances are one thing, as long as they are over a few
thousands, on a modern CNC do not seem relevant to me. If you have a
tolerance of .05" or a tolerance of .005" my cost will be the same. I
am not hand filing down to a size. The machine and process will come
out more accurate anyway, unless there is an issue with holding the
parts, or there is a ridiculous amount of steps to make the part. If
the tolerances get smaller than .002" then they can become a factor on
a small part. .0001" gets more and more expensive. But loose
tolerances don't help me out since the machine is making the parts to
a basic tolerance no matter what anyway.

Many parts I make from thicker material, then flip them over and
machine off the bottom.
If the top has a feature I can grip easily, they get flipped over into
standard jaws. Otherwise one of the quickest ways is to cut a custom
set of soft jaws to clamp the top of the part into while the bottom is
milled off.
You can also cut reference surfaces for secondary operations that get
milled off in the final operation.
An example of that was set of custom roller rockers for a hot rod
valve train.
The first operation cut out the basic shape from thicker material, and
also cut some extra angle surfaces on the extra material. The second
and third operations were at odd angles for the push rod screw and
another hole at an odd angle. The last operation cut the built in
fixturing off of the final part. Leaving someone wonder how much magic
custom tooling it took to make. Not much, it was built in, and
disappeared at the last operation.
For small runs I don't like to be making little fixtures and screwing
parts down If I can slap them into soft jaws, or leave features on the
partially finished part that will be my fixtures. The other advantage
is in and out of soft jaws is really fast. And with a location feature
made in the first operation, tolerances do not add up so much from the
needed clearance of a secondary fixture.

Getting back to cost, small features are costly. I just made a batch
of parts that were 4" by 1.75" the outside cut really fast with a 1/2"
endmill. But, there were tiny little slots, that needed a 1/16"
endmill. Those little slots cost more than the rest of the part, and
the material.

Thank you very much guys!!!

that was a refreshing treat to have in-depth responses that really
shed some bright light on the situation!