Cnc wrapper/4th axis help

[topchippy1]

I have the wrapper programme...all good..got code in and toolpath up...but when I set the zero to the work piece and run the a axis rotates...the z goes up..( should go down) and the x is stationary.....am or how do I set the zeros to start cutting...oh by the way..I have only owned a cnc for 4 weeks!!!
just to add...on looking at the code I notice that the z code is all plus and not minus....so instead of the cutter dropping in 1.6mm it raises up 1.6mm....what am I doing wrong

[adprinter]

It depends..... if you are using the A axis (4th axis) with tool path generation completely from CNC Wrapper, then the "correct" Z zero should be set to the center of the part. If you are setting the Z zero, by jogging your machine down to the surface of your work piece and resetting Z zero, this is WRONG! But, as I said, it depends.... If you are using CNC Wrapper to convert g code generated by another program, to WRAP it around a cylinder, then you SHOULD set the Z zero to the surface of your work piece. 4th axis tool paths are an entirely different animal to get your head around. But basically, it functions similar to a lathe. (The Z Zero on a lathe is always the center of the stock). The programmed diameter of the work piece stock, is what CNCW is working from. Therefore, if you have for example a programmed stock diameter of say 2", and you have jogged your tool down to touch the surface of your stock, and reset Z zero, then subsequent Z moves WOULD move UP instead of down! As CNCW is trying to cut the radius of the stock relative to the stock's CENTER. (Which will always be a positive move- if it were negative, it would mean that the tool had to plunge into your stock completely PAST the centerline of the stock!). And since you probably have your stock mounted between the headstock and the tailstock, would result in your work piece being completely severed between the headstock and tailstock of your lathe (4th axis assembly). I would recommend learning to generate a tool path, such as engraving your name for example, in another program such as LazyCAM. Get that working successfully, on a FLAT piece of stock. THEN save that tool path g code file. Import it into CNC Wrapper, and CONVERT it for "Wrapping" around a cylinder. The trick is, you have to get your math EXACT in terms of the Y axis limits of the FLAT tool path, which will be converted into A Axis moves in CNC Wrapper. I.E. the Circumference of your A Axis work piece must EXACTLY match the measurement of your Y tool path limits of the FLAT g code tool path. If it is not an "exact" match in measurements, the only thing that should happen, is that it will engrave your name all the way around the cylinder, until the first letter meets up with the last letter. If the circumference of your work piece cylinder is SMALLER than the actual Y measurement, then the work piece will continue to rotate until the last letter engraves on top of the first letter. If the circumference is LARGER than the actual Y, then it will leave a GAP between the last letter of your name, and the first letter. As I said, 4th axis is a different animal to learn. Especially if you are new to CNC. I would first concentrate on mastering 3 axis tool path generation. THEN try and tackle 4th axis later, once you gain a better comprehension of what's going on. It will get easier to understand. Hope this helps!

[adprinter]

I have the wrapper programme...all good..got code in and toolpath up...but when I set the zero to the work piece and run the a axis rotates...the z goes up..( should go down) and the x is stationary.....am or how do I set the zeros to start cutting...oh by the way..I have only owned a cnc for 4 weeks!!!
just to add...on looking at the code I notice that the z code is all plus and not minus....so instead of the cutter dropping in 1.6mm it raises up 1.6mm....what am I doing wrong

After I replied to your post, I went back and read it again. The standard for XYZ axis should be: X= moves which are left and right Y= moves which are toward or away from you Z= moves which are up and down. It is important to note, that in my first reply, this was the thinking applied. But after re-reading your post, I realized that you seem to have your axes set up opposite of "standard" I.E. you seem to be applying the "toward or away from you" movements as X, instead of Y axis. Which WOULD result in a "Stationary X axis" if the axis you have set up in CNC Wrapper is in fact the X axis. The references I made in my first post to Y axis movements, assume "toward or away" movements (the tool path which is to be converted by CNC Wrapper to be "Wrapped" around your cylinder).
To avoid confusion, it may help you to think about looking at a sheet of notebook paper. With the page oriented with the narrow width facing up and down, and the wide width facing left and right. The lower-left corner of the page is generally where the industry standard for Zero is located. (although it can actually be set to anywhere you like). If you will simply orient your machine in a similar manner in relation to the computer you are using for machine control, it will help you to avoid any confusion. At that point, jogging the machine left or right on the computer keyboard's arrow keys, will match what you see physically happening to the machine itself. (X axis movements). Or jogging the machine up or down on the computer keyboard's arrow keys, will also match what you see physically happening to the machine itself. (Y axis movements). The page up and page down keys on the computer keyboard will raise or lower your tool on the machine itself. Of course, it is ALL relative to your particular configuration. The above info assumes a machine with a moving gantry. If your machine utilizes a fixed gantry, with a moving table, things are actually REVERSED! But the visualization still applies, as it is all relative to the tool's physical position. Once you gain a firm comprehension of all this, it does get easier!

[topchippy1]

I have the machine set as y back and forth, x left and right ,z up and down, I have done quite a bit of 3 axis work and got on quite well...all beit for a few teething probs regarding feedrates...but not bad in general...I now understand that the z zero should be at the centre of the workpiece...so if I have a piece of stock 70mm , i can touch the tool to the piece and, am I correct in saying i can manually type in a value to the z dro of -35....thus achieving zero the centre,.....only prob is, I have tried this but every time I go to start the dro resets back to zero....am I missing something...by the way...thankyou very much for your input...has helped me understand it a lot more

[ger21]

It would be 35, not -35. Right? Be sure top hit enter after typing the value in the DRO.

[topchippy1]

Ahhhhhh....excellent...that is what I was doing wrong...or not doing as the case may be...hitting enter after typing in value....and yes..thanks for pointing out it should be 35.00 and not -35.00...goona go play now!!!