Setting and programming Part-Zero

[rtzic...@gmail.com]

Hello,
I am new to the PocketNC and would really appreciate some guidance. I have a few questions in regards to work offset and programming of parts.

1) How do you find the X0, Y0, Z0 on your part once you mount it to the B-table?

2) Where would you enter these values (I am assuming perhaps in the G54-G59 offset registers).

3)I use Mastercam for programming. When creating programs, Can I place my part zero anywhere on the part, or must it be set to exact center of the work piece?

4) Is there any documentation or step thru examples on how to do these things. I have seen the documentation for setting the Z tool length which I am assuming is the C/L of rotation for the Z-axis.

Any help or guidance would be greatly appreciated.
Thank you
Richard

[Pocket NC]

Hi Richard,

1.  The XY zero of the machine should always be the center of rotation of the A and B axis.  This is how your machine is setup when we ship it, so you should not have to worry about finding this point on the machine.  You will want to find the distance from your part edge to the machine zero.  To do this, jog the machine until its close to a surface then use a set of feeler gauges to get the distance from tool edge to part edge.  You will now adjust the distance from your part edge to your origin in Mastercam by the distance you measured on the Pocket NC readout.  Take a look at how users setup the a cube for the Pocketnc using Fusion 360,  The software is different, but the concept is the same.  

2.  The Values you measured should be the amount you offset a part from the origin within Mastercam.  For example, if you measured the edge of your part and it was 1" offset in X, you would want to place that same edge 1" form the origin in Mastercam.

3.  Unlike 3 axis machining, the origin cannot be anywhere on the part.  It must be at the center of rotation for the machine.  We show this in our Fusion tutorial be sure to have a look.

http://www.pocketnc.com/part-setup

Thanks,
Matt

[rtzic...@gmail.com]

Thank you Matt for the explanation and the quick response. So to be clear, we do not use any type of offset (G54 etc.) when setting up the part origin on the machine, instead, we must physically move our CAD model to match where the actual part is located in relationship to the machines 0,0,0. Correct?

So if multiples of the same parts are to be made, we must shift the CAD model for each part unless we can figure out a way to mount each part so that's it's locations is repetitive to the 1st part we touched off on?

Does the same hold true for setting the Z-axis for the tool length? Is that what that sheet of paper explains when using the supplied 1-2-3 block? Are we calibrating the tool to the centerline of the A and B axis intersection point, then touching the face of the part in the Z-axis to find the offset difference from table centerline, and then shifting our CAD model to to match where the physical Z axis location of the workpiece I relation with 0,0,0 of the machine?

If the above is the case, maybe I will have to build a little part mounting block that is permanently mounted to the 0,0,0, of the table similar to how companies use a 3R fixture system where a piece of stock can have a dowel hole drilled in it for locating the stock on the 0,0,0 point of the mounting block and held with some adhesive or a mounting screw.

Kind regards Richard

[Pocket NC]

Thank you Matt for the explanation and the quick response. So to be clear, we do not use any type of offset (G54 etc.) when setting up the part origin on the machine, instead, we must physically move our CAD model to match where the actual part is located in relationship to the machines 0,0,0. Correct?

Correct

So if multiples of the same parts are to be made, we must shift the CAD model for each part unless we can figure out a way to mount each part so that's it's locations is repetitive to the 1st part we touched off on?

If your are running the first operation, just have the program account for the extra stock or the largest piece of stock.  If its a second operation, a fixture will keep you from having to adjust the part each time.

Does the same hold true for setting the Z-axis for the tool length?

No.  users will need to set up each tool in the tool table, here is a link to that (http://www.pocketnc.com/tool-length-offsets-new-spindle)  

Is that what that sheet of paper explains when using the supplied 1-2-3 block? Are we calibrating the tool to the centerline of the A and B axis intersection point, then touching the face of the part in the Z-axis to  find the offset difference from table centerline,  and then shifting our CAD model to to match where the physical  Z axis location of the workpiece I relation with 0,0,0 of the machine?

The tool is being set, using the tool table, to the centerline of A.  The part that physically sits on the table has a XYZ location to the machine G54 and that is the only thing that gets offset within the cam program.  The machine will handle tool length compensation using g43 but you don't need to worry about that.  Just getting the tool lengths correct in the table.

In the Fusion360 tutorial, we recomend users put the stock material in the vise that comes with the machine.  This vise has dowel pins for location, so it gets the user very close to the desired location (usually within a few thousandths)

Thanks,

Matt

[rtzic...@gmail.com]

Thank you Matt.....your customer service is EXCELLENT!!! and your help is greatly appreciated. I ordered the stand alone HDMI interface kit from your web site store. It should be in next week. Once I get it all hooked up, I will follow your instructions.
Thank you
Richard