[vonnieda]

Hi all, I have a few total newbie questions so I hope you'll bear with me.

First, a little background: I have a Taig CNC mill that I bought about a month ago and I've been learning all I can about milling. I am totally new to milling and metalwork in general.

What I'm having trouble with, I think, is in regarding to layout, mounting and clamping. I'd like to know how other folks would do the following operations.

I want to make a basic part from aluminum. It's a 4" x 4" x 0.5" box, rounded outside corners and an interior 3.5" x 3.5" x 0.4" pocket. I'd like to run the mill over all sides of the box to produce a nice clean surface.

I've come up with a CNC program using CAD/CAM software that will do these operations, but I have not figured out how I should be mounting the stock, or whether I can expect to do all the operations in a single mounting or if I need to plan to move it around.

So, just to help me get a clue I'd like to ask you to describe how you would mount and setup stock to cut this thing out.

Some thoughts I've had are: Do I use thicker stock than I need, clamp it towards the bottom, contour high and then cut the piece out from the bottom in a final pass? Or do I have to clamp it one way, contour two sides and then clamp it again to contour the other sides? How do I safely remove the finished piece from the stock?

I know this is super basic stuff, but hopefully someone is bored enough to respond

Thanks,
Jason

[tobyaxis]

I know this is super basic stuff, but hopefully someone is bored enough to respond

Thanks,
Jason

That's pretty funny

You want to clamp and machine your part using the least amount of operations and set-ups. Larger stock is a good idea and will reduce your project to two operations.

Depending on the size of your vise (I usually have Kurt 6, 8 , and 10 available) do what was suggested earlier. Hold onto a good 1/8 of stock at the bottom and do the Face, Profile, then the Pocket.

Flip for Op2 to Face the bottom.
First Snug lightly, Now tap lightly with a dead blow hammer to seat the part firmly on the parallels/soft jaws. Check to see that you can not remove the part pulling with your hand. Be careful not to cut yourself! Also be mindful because the floor is pretty thin now. It is best to use a smaller tool diameter at lower rpm and feeds so you don't have any large chips or chunks flying off at you. Chatter is also a concern my suggestion of low rpms and feeds.

Check to see if you thickness is correct and if so remove. If not take another skim cut.

Cheers

[vonnieda]

That's pretty funny

You want to clamp and machine your part using the least amount of operations and set-ups. Larger stock is a good idea and will reduce your project to two operations.

Depending on the size of your vise (I usually have Kurt 6, 8 , and 10 available) do what was suggested earlier. Hold onto a good 1/8 of stock at the bottom and do the Face, Profile, then the Pocket.

Flip for Op2 to Face the bottom.
First Snug lightly, Now tap lightly with a dead blow hammer to seat the part firmly on the parallels/soft jaws. Check to see that you can not remove the part pulling with your hand. Be careful not to cut yourself! Also be mindful because the floor is pretty thin now. It is best to use a smaller tool diameter at lower rpm and feeds so you don't have any large chips or chunks flying off at you. Chatter is also a concern my suggestion of low rpms and feeds.

Check to see if you thickness is correct and if so remove. If not take another skim cut.

Cheers

Thanks very much for this response! This really clears a lot of things up for me!

[tobyaxis]

Thanks very much for this response! This really clears a lot of things up for me!

Your Welcome!!

Be sure to post your results or more questions if you have them.

[One of Many]

Thanks very much for this response! This really clears a lot of things up for me!

You could also do a process known as trepanning.This involves using a larger piece of stock and cut your part out of it in one setup. The clamps must be clear of the path for the outer cutter profile.

Use some hold down clamps to clamp the stock on top of a sacrificial piece of MDF so you don't cut into the table. You will be clamping both to the table at the same time.

Set your origin in the pocket center or where ever convenient. Mill the pocket complete, then groove mill the outer profile a bit big at a depth about .010-.015 from breaking through the stock. Then do a finish pass around the profile to size. One last pass to cut through or, thin out the remaining bottom material enough to pop it out of the stock with a rubber mallet. You can do the last 2 passes there in one. The concern is if the part comes loose, it can be left with a cutter mark or uncut tang at seperation.

DC

[escott76]

Another option is "heat activated clamping compound", which can be found at McMaster Carr amongst others. Part number 50245A21 there. Basically a fancy double stick tape that releases at ~200 degrees. You could face one side, then heat and stick it to another piece of stock, cut the outside and the pocket, and then heat to remove.
I second the option given of cut the outside and pocket, clamp, and skim the floor. When the floor is too thin to behave well the adhesive method works well as it holds the thin flat bottom from flexing and pulling up into the cutter.

[vonnieda]

Set your origin in the pocket center or where ever convenient. Mill the pocket complete, then groove mill the outer profile a bit big at a depth about .010-.015 from breaking through the stock.
DC

This brings up two more questions:

What do you mean by groove mill? Is that just running a slot around the outside of what I'm trying to cut out? i.e. literally just milling a groove?

And regarding origin, when doing stuff with CAD/CAM, is it generally normal to have the drawing centered at 0,0 and then you just decide where that is going to be on the stock?

Thanks again for all the answers, this is excellent information.

[tobyaxis]

This brings up two more questions:

What do you mean by groove mill? Is that just running a slot around the outside of what I'm trying to cut out? i.e. literally just milling a groove?

And regarding origin, when doing stuff with CAD/CAM, is it generally normal to have the drawing centered at 0,0 and then you just decide where that is going to be on the stock?

Thanks again for all the answers, this is excellent information.

Groove mill can be one of two things. A woodruff cutter or mill/drill type tool.

As for Part Origin most use the Too Left Corner between the Hard Jaw on the Vise and the Work Piece Stop on the left. It is then programmed X+ Y-. It makes it easier for the operator to see the origin.

[One of Many]

This brings up two more questions:

What do you mean by groove mill? Is that just running a slot around the outside of what I'm trying to cut out? i.e. literally just milling a groove?

And regarding origin, when doing stuff with CAD/CAM, is it generally normal to have the drawing centered at 0,0 and then you just decide where that is going to be on the stock?

Thanks again for all the answers, this is excellent information.

Yes, trepanning is cutting a groove to free the internal section from the outer section, without turning all the excess into chips. The other benefit is simple clamping, doing as much as possible to the part geometry while it is still clamped, reducing secondary setups and hard to hold operations.

We vacuum hold 4'x12' sheets of aluminum using the same method on our Komo routers.

The origin can be anywhere convenient. For one-off parts, I prefer to locate my origin on the part. If I must indicate the part and know the distant to some other origin, I might as well use the indicated position on my part as my origin and forget some other point out it space that may or may not be relevant since I move the vise often, change the jaws etc. Besides, I do my own geometery, post my own progarms and run the part. When someone else is doing the program, they might get anal about where the origin should be.

In a production run environment, using a set of soft jaws or nesting fixture, then do what makes sense and use the origin you are given for a repeatable setup used in the previous run.


For your small part, as long as the part is within the blank area you desire to take the part out of, it isn't critical. Clamp it to the table, jog near center, set x,y zero and go. If you find you want to cut another, jog over to the center of where you want next part to be, reset the origin and go.

DC