As a newbie, I'm finding the forum threads incredibly helpful! I've also been watching Darrell Holland's VMC DVD course.

I have a question that, although basic, I can't seem to find an answer on the forum:

When you have your CNC program/code ready for the part and you put the part in the vice, how does the mill know where the part is located? I.e. each time you put a part in the vice, I'm sure it's going to be, at best, a few thousands left or right of the last time...

Thanks!

If you need the part located so accurately, put a rigid "stop" on one side and consistently place the part against the stop. The part must still be positioned the same way every time. Different people will have a variance of ~.001" due to differing hand pressure while closing the vise.

This is a fancy one. Some clamp to the vise fixed jaw. They are available from MCS and Enco. Often, shops make their own to suit their needs.
http://www1.mscdirect.com/ProductImages/8293600-11.jpg

The mill knows where the part is located when you have used an edgefinder. If you want a consistant zero, you will have to use stop like the one Caprirs posted.

You use a stop like caprirs showed so that each part is put in the vise in the same position.

But before running the first part you have to enter what are called Work Coordinates, or the Work Zero, into the machine and this is what The Blight is referring to in mentioning an Edge Finder.

Your CNC program is based on a zero point somewhere on the part, this is the Work Zero; it could be a corner of the part. The machine operates using machine coordinates and when the machine is homed or zeroed it automatically moves to the zero point in these coordinates. Normally this means the table moves as far forward as possible and to the left as far as possible with the spindle as high as possible. By convention all machine motion from this point is considered negative motion on any axis and while the table actually moves for X and Y we say that the spindle is moving negative X when the table is moving toward the right and similarly when the table moves away from the operatore we say the spindle is moving negative Y. Z is easeir to picture; the spindle moving down is negative Z.

So if your part Work Zero is at the corner it is necessary to know the location of this corner in machine coordinates; that is the X and Y coordinates when the centerline of the spindle is above this point. These are the Work Coordinates which are entered into a table in the machine controller and called G54, G55, etc. The most common default choice is G54.

The Edge Finder, or some other method is used to position the spindle at the Work Zero in order for these coordinates to be located. Basically with an Edge Finder you have a probe with a known diameter that you bring into contact with the edge of the part and then move the machine an additional distance equal to half the diameter so now the center is in line with the edge. Do this for both X and Y and you have the center of the spindle over the corner.

The Z coordinate can be located either by using a Work Coordinate entry or by using a Tool Offset. The important thing is that you need to know the position of the tip of the tool relative to the top of your part. The machine Z coordinate for this is going to be different for different tools because they will be different lengths so Tool Offsets are used for each tool but a Z Work Coordinate may also be used in combination with Tool Offsets.

To determine the Tool Offset the tool is brought down until it is just touching the top of the part and the value of this location in machine coordinates on the Z axis is entered into the Tool Offset table in the machine controller.

Now your machine "knows" where your part is.

I apologise if this explanation is more long-winded than you where looking for.

You can also use one of these 3D tasters (edgefinder with 3rd axis)
This one costs about $160

You can also make one yourself as I'm doing. I might be able to post some drawings of it in about a month or so. It's made of stainless steel and uses a regular dial gauge. All the tolerances are H7, so you need some good machines to make it, but it should work quite nicely. Not as accurate as one you can buy, but I guess +/- 0,01mm (0,00039) is do-able.

http://www.chronos.ltd.uk/acatalog/3DDL.jpg

To determine the Tool Offset the tool is brought down until it is just touching the top of the part and the value of this location in machine coordinates on the Z axis is entered into the Tool Offset table in the machine controller.

.
Unless you have a tool presetter:
http://www.inspection.ie/shopping_admin/product_details/product.cgi?product=1PS&cat=Tool%20Presetters&sub=Tool%20Presetters--Trimos%20Tool%20Presetters

They measure both length and radius of the tool.
All you have to do is read the meter and write the value in Tool offset.

Correct, Tool Setters and Probe Systems can be used. I was trying to answer in what appeared to be the context of the query in an introductory sense. It does not matter how you do it you are telling the machine the location of a reference point on the part. I think for a novice it is better to answer questions at an introductory level and not expect them to know the jargon of the trade yet.

Ok, you have a point there.Your explanation was perfect,I just added an another way to do it.

Thanks! You guys rock.