How to you zero to an A Axis?

[bralwel]

I'm hoping someone here can help me on how to zero to an A-axis. the A-axis is parallel to the X axis. I got how to zero in the y direction using an edge finder, but how about the Z axis? I've been using a feeler gauge, but there has to be a better, more accurate way. Anyone have any experience in this?

[HuFlungDung]

It might be convenient to zero your Z axis at the center height of the A axis centerline. However, the actual zeroing of the A axis would mean finding some kind of switch home on a cnc controlled A axis. This would be a built in function of the controller for the A axis.

It is also possible to offset the start position of the A axis with a degree entry in the relevant work offset table. If your part has an identifiable feature on it that you need to indicate into position, then this feature will have an angle that you should know from the print. Note the difference between the A display current position and what you intend that the current part position should be at, and enter the difference in the work offset that you will be using.

On a manual A, you just turn it to 0 degrees to start.

Not sure if that helps or not.

[little bubba]

On our Fadal, the body of the 4th is pretty much dead nuts ground square, and I know that the center of the fourth is 3.984" from the top of the 4th. That is what I use. If the top of your 4th is crap, then find the center distance to the table, real easy using an indicator and a gage pin. Now write that number on your machine somewhere in paint pen with death threats to anybody that erases it, or I guess you could write in the front cover of a manual. On our Fadal on the sheet metal covering the spindle in blue paint, big letters, it says "3.984 center of 4th to top".

Knowing that reference of center to some standard (table or top of the 4th), you will now have a reference and never have to try and set a tool off of a round object again.

[bralwel]

Thank you both HuFlungDung and little bubba. I'm definitely a newbie to all this. I like the idea of measuring from the table top to the centierline. Unsure what the dial gauge and indicator pin are. How would I use these.

[little bubba]

The indicator and the gage pin. Simple, chuck up the gage pin your 4th axis (if it has a 3 jaw or a collet nose on it). Stick an indicator in a tool holder, stick the tool holder in the spindle. Zero off of the top of the gage pin, check the 4th for runout while your there. Take note of your Z axis position, now use the indicator to pickup your table or the top of your 4th. Now, simple math, the difference between the two Z axis position s, plus or minus the radius of your gage pin (depending on weather you went up or down) the poor mans cmm. Of course you didn't say what machine this was on, so if its a manual without a readout for the quill, then its pretty much a moot point, though a height gage on the table could tell you the same thing.

[bralwel]

Ah, yes, I probably should have mentioned this is a MAXNC. But now that I have the idea, I can go from there.

thanks again!!

[bralwel]

Hit post too soon. Where is a good place where I can get a Gage pin?

[little bubba]

A gage pin comes in a set of pin gages, any piece of round metal, that is consistant and you know the diameter of will work. I you don't have a set of gages, an endmill shank works just as good, nice and round and a fairly tight tolerance.

[sanddrag]

I'd move the Y such that the Z was directly over the centerline of the A, then I'd just come down on top of it with a pice of paper between the part and the tool. Then I'd move the paper back and forth with my fingers while SLOWLY advancing the Z down in the smallest possible increment. When I feel a slight bit of resistance in moving the paper, I'd remove the paper, move the Y so that the tool is away from the part, then move the Z down the thickness of the paper, then set the offset.

But that's me.

[warpedmephisto]

True, using the paper/feeler gauge method works well on individual setups, but sometimes its nice to know for sure how far the centerline for the 4th axis is from either the top of the 4th axis body, or up from the XY table plane. That way when you write your program, you can always zero the 4th axis on centerline of the part, assuming that the part has an axial centerline, ie: its a cylinder shape. However, the feeler gauge method might be more helpful when doing square or odd shaped parts that sit offset from the 4th axis' centerline or parts that have no axial centerline.

[bralwel]

I'm using the 4th axis as a way to index. When generating the G-code, I'm setting zero at the center of the item and then rotate around the center point, so I am looking at it being in the dead center. Item is a cube shape and I'm machining each side, so I'm machining one side, rotating 90 degrees, machinging next side, rotating 90 degrees, etc.

How about this? If I set up the Y axis on a pin using an edge finder and zero it out in this direction, then bring the mill bit down exactly on the top of the pin, loosen the bit so it sets directly on top of the pin, then tighten it up. From there, I would think it would be exactly the radius of the pin to the center. Would that work? Or am I doing this the hard way?

[warpedmephisto]

I don't really see a problem with doing that method, but if its just a simple cube with 90 degree rotations, you could just use a depth stop in your vise and machine it just using the XYZ axes. Though using a 4th axis would be higher on the "cool" scale I suppose.