[bloefeld]

Hi,

I have zero experience with milling, cad software and cam software. I am an inventor and work in composite materials for the most part.

I have done a bit of robotics and some machinery design and implementation in a production facility that I designed and built for a product that I invented.

During the plant build I did a little bit of milling work on a gear-head mill to make adapter plates and the like. I enjoyed the work and thought I would explore it more.

I purchased a HAAS Toolroom Mill TM-1 and thought I would figure it out.

I then had a design problem that I could not sort out by using AutoSketch. So I bought Alibre Design to get started in parametric modeling. It works OK but is sometimes surprising. The price was pretty good and did not require the investment of Solid Works or Solid Edge.

I then needed to make the parts I had designed on my mill. How hard could that be? So I purchased Alibre Cam and thought I just had to diddle around with it a bit and I could clamp the stock in my mill and turn on the machine and it would, you know, cut away all the stuff that didn't look like my part.

Incredible learning curve later I actually managed to make some sort of part that looked a lot like my drawings. In the interim I was close to going postal.

Now I am getting serious about making parts that are accurate and are well finished.

I am taking courses and getting advice from anyone who knows more about the topic than I do.

My question, and I do have one is this;

If I draw a part that needs to be machined on two sides and I fit my box stock in my cam program so that the least amount of material is cut from the bottom of the part and then I turn the part over, where should I touch-off the tools?

It seems to me if my box stock is not entirely accurate the part will cut too large if I touch of on the actual top of the stock. If that is the case, should I touch off on the bottom of my vice and add more or less the height of my actual stock, will my part cut closer to my drawing than if I touch-off on the top?

Cheers,

Bloefeld

[Matt@RFR]

Now that's what I love hearing... a person not originally from this field finding out that this CNC stuff isn't as easy as it looks! Good for you, now spread the word. (Like the guy who designs a 4 axis, 2 setup part and is furious with you for wanting anymore than $50 to make ONE)

As for your question, the answer is all of the above. Sorta. If you have the luxury of measuring the "box stock" (which I'm taking to mean raw material) for thickness, and it is consistent, you can program your second op accordingly, then touch off on the top of the stock. Or you could touch off your vice bed/table/sub plate/parallels and be much more accurate, while not having to worry about material thickness.

A third option for second ops is if you're using soft jaws, I will generally program my work offset for the upper left corner of the jaws as XYZ zero. That way you don't have to worry about material thickness AND it's much easier to get the X and Y offsets when dealing with odd shaped parts.

Bottom line... if it works, it's right.

[cadman@teluspla]

I would agree with matt @RFR about soft jaws
if you want repeatability that is the way to go.
I would also add that when you cut your soft jaws machine an area where you can touch off for xyz when you go back to that job and reinstall the jaws on your vise you know where they are located.
I do this because we take a skim cut off our soft jaws any time we go back and setup a job we have done before.

[bloefeld]

I knew the learning curve is going to be steep and I am very glad I found this forum. An easy exchange of ideas and answers to questions it great.

I have found the most confounding thing about my CAM software is the (to me) odd way it set-up 2 1/2 axis versus 3 axis operations and this is a big cause of issues relating to touching off and accuracy.

In Alibre CAM all machining is done parallel to the xy plane. In 3 axis mode it 'knows' where the part is relative to the xy plane and takes into account the height of the Box Stock (the imaginary starting block of material to be machined) from the most upper point of the part. In 2 1/2 axis machining you have to locate the top of your part relative to the xy axis and then add the top of your box stock to the point you are going to get to as you do a facing operation.

Why they designed it this way is a mystery. Because I have not actually used or seen other CAM systems up close I have no idea if that is just the industry standard or if MecSoft is insane

Thanks for the help. The curve is getting a little less steep thanks to guys like you.

Cheers,

Bloefeld

[Paul_S]

Generally I have all the tools to be set off to top of the stock. I use a 1.000" alumium block like a go nogo gage. (So not to lower the tools directly on the part or on the block.*) Use the z tool set option on the control for each tool. Then go in and add -1.000 to each tool length. You can do this in the wear column.

If I'm going to machine two sides in one setup, I put the second side in a second G offset. First side G54. Second side G55. and place any difference for the Z value in the G55 Z setting.

For example: If the first side the hight of the machined part finishes, lets say at 1.25 inches. The second side the finish width is to be 1.225. Then in the Z value for G55 I would place -0.025. The G54 Z value being 0 (zero.)

Any questions?

[The go nogo method. You jog (.010 setting) each tool about 1.00 above part. And lower it until the 1.000" block will not slide under the tool. Then rase it up .010 at at time, until it goes under the tool. Then lower it just .010 so the block does not go. Then change the setting to .001. And rase up to tool .001 and check. Repeat. When it goes under the tool. the hight is there. If you want to set it to .0001 repeat the method using .001 to .0001 setting. Typically .001 is close enough.]