Indexer mistakes

[blackhawk]

Well, it has been 2 weeks since we have had a new indexer post. I will break the ice with some lessons learned after my last project.

I wanted to make a sample table leg to show potential customers. I drew up a 30 inch long leg with different contours including a tapered section. I use Aspire for my toolpaths and it has worked great so far. I go back to Randall's tutorial for help all the time. The leg turning went pretty smooth. In my great wisdom at 9:15pm (45 minutes before my favorite TV show), I decided that I would V-carve my company logo/initials with raised letters in a pocket along the tapered section of the leg. This easy task couldn't take any longer than 30 minutes, I said to myself. This is where my lessons/mistakes began.

#1) Letters v-carved on a turning will be backwards if your +/- in front of the B-axis unit value is backwards. Luckily, I caught this before I cut very deep into the leg. (Anytime, I have a 50/50 shot at getting something right, I lose. This is why I was banned from callling the toss for my softball team.)
#2) Your endmilll will cut through whatever is in its way, when you forget to adjust your Z zero routine for the center of the stock. I have a spot on my lathe that I zero to with my plate, but after I zero there I have to move the Z to .625 and then do a "ZZ" command. This sets the bit to the center of the stock. I zeroed to my plate, but forgot to do the zero adjustment.
#3) V-carving on a taper ends up being a little distorted. After I cleaned up mistake 2 and 3, I finally tried the raised letter V-carve in the oval. The letters were a little skinny in places and the distortion from the taper made several edges just break off. So now I had a .200 deep pocket with a mess of letters.
#4) When making a pocket on a taper (to clean up my mess), a standard flat endmill does not leave a good finish. If you think about it, the flat end of a regular endmill will create steps in the pocket, since you are not on a flat plane. I switched over to a ball nose endmill with about a 15% stepover and the pocket came out very smooth. Hardly any sanding.

Long story short, after cleaning up all my mistakes I had a .300 deep pocket on my leg with nothing in it. I then just decided to do a standard V-carve into this pocket with my company initials. Again, the letters still have a little distortion on the taper, but it looks OK. I know someone will say, "wow, that is a deep pocket that you cut just to carve those letters into". I then have to decide whether or not to admit to my mistakes, so that I can defend my pocket depth.

Oh yea, I got done fixing all this mess about 11:00 pm. Missed my show, but luckily hit record on the old school VCR in time.

[srwtlc]

I hate days like that. Glad to know that someone else has a 100% chance of the wrong side of 50/50! ;)

Have you thought about adding the z adjustment and a ZZ to the end of your zeroing routine file and "save as" Indexer Zzero to another Custom Cut #?

Scott

[dana_swift]

Brad- thank you for the info. I thought I had made every mistake in the book, however some of those are new.

Mistakes can be creative in that way..

D

[myxpykalix]

Brad,
you know what i took away from that long explaination? You never told us what your favorite show was?

I too was looking for a quick simple way to Z zero to the center of stock and had read posts about Z'ing to a part of the indexer and then offsetting and that always made me concerned so i did the simpliest thing i could think of.

I measured from the bed of the indexer to the center of the dimple in the end of the shaft and cut a 2x6 to that height and simply use it as a jig. I set it down in front of the chuck do a C2 and its done. No offsetting, no remembering (or forgetting) and your done.
I had a picture of it somewhere but can't find it, but this one should illustrate it.

[blackhawk]

Scott and Jack - Those are both good ideas to prevent the Z zero mistake again. I definitely need to do one or the other.

Another interesting thing came up when I built my own indexer using a Rikon lathe. I first tried zeroing with my plate setting on top of a metal part of the lathe. When I ran the z-zero routine, the bit would touch the first time, then retract as normal. On the second touch off, it would start to go down, stop, and give me some random zero setting. I figured out that I had to add a piece of nylon to insulate the z-zero plate from the lathe. With the nylon in there, everything works as normal.

[myxpykalix]

I think about that all the time because i have metal clamps i use to hold down my material and i am afraid by touching one of them during the C2 process might give it a false reading so i am carefull in that regard.

However you description of adding a piece of nylon to insulate made me think of something. How thick is this nylon? If you added it to the bottom then if you don't adjust your thickness setting for the aluminum plate then you are going to get incorrect readings. If the nylon is the thickness of a sheet of paper i guess that might not be a problem.

[widgetworks_unlimited]

I think of my machine as several cutting areas stacked together. I have the indexer area, the vertical/dovetail area, the 4x8 vacuum table area, and the 1x8 long fixture clamping area.

I setup a separate post processor for each area that knows how to offset x, y, and z zero from the main vacuum table settings. That way, I always zero my bit to the same spot on the table, and the prox switches work for homing 0,0,0 for all areas - no extra setup needed.

One of the benefits to this is that all of my design files are drawn at 0,0 and once the cut file is saved with the appropriate post processor, I don't have to worry about forgetting to manually reset all this stuff.

My post for the 4th axis takes things a step or two further...

It automatically eliminates the potential for cutting into the chuck while I move the spindle for tool changes.

I also built in an automatic square stock to round blank routine, so I didn't have to remember to add that step while creating the cut files. Unlike the Vectric option, I use all climb cutting for blanking, which eliminates most of the huge splinter/tearout issues that are "special" to 4th axis turning. I turn the octagon shape into a cylinder using a spiral wrapped cut at jog speed, which eliminates the need for ramping. It's much faster than Vectric's raster method. (You can compute the dimensions of the square stock automatically inside the PP based on your model size, so you don't make a mistake doing the calculations.)

I need all the dummy proofing that I can get!

[Brady Watson]

For Zeroing the Z with the Indexer, I measured from the top of the tailstock flat area to the center of the live center point...Using the Bot itself and Fixed mode in Keyboard Mode to get a precise measurement between the two.

I then put a piece of 2" wide masking tape on top of the tailstock to electrically insulate it and hacked the Zzero.sbp file to account for the offset distance between the flat on the tailstock and true center. Works really well.

-B