What the heck is going on??

[myxpykalix]

I have rounded square stock before with no problems, so i don't know whats up!

I used the indexer virtual tool to round square stock. My intent was to take a 2" square and take it down to 1.75" round. Here is how i filled it out in the boxes (interface1.jpg)
It took a total of .50 off the square when according to the interface it should have only been a total of .25 right?

Then i started a second file this time i filled it out according to (interface2.jpg)

It starts out at .166" and tapers down to .93.
I centered and Zzeroed the bit to the center of the chuck before hand. The indexer has probably 10-20 hours on it so i don't think it is mechanical with the indexer.
So what would make it just taper like that?


8500

8501

8502

8503

8504

[waynelocke]

Did your bit slip? Check to see if the bit is still zeroed to the center.

[cmagro]

Jack,

First thing to check is if the center at each end is the same. If you have spur put it in the head. I use my v-groove bit and line it up to that at the correct height..then move the bot along the x to the tail and see if the point of the v-groove bit is at the same height as the live center (or whatever you are using at the tail end).

Over a 32" length if you are just 1/8" off your blank would be off 1/4" from head to tail.

Also remember the downward pressure on your material the bot will place. The material strength, length of stock, diameter and how much material you are taking off at a time could easily cause this problem (to some extent).

The fact that it starts out correct (close to the head at the strongest point) and then gets weaker and thinner makes me think this is highly possible.

And is your blank centered correctly..you are working with a small diameter here....

A combination of these factors is most likely the problem.

Always try to look at the code...even if you think you don't know what you are looking at..read line by line and you will start to visualize what is happening..

Christian

[myxpykalix]

Christian,
Here is what i have checked. I took the chuck off the shaft of the indexer. There is a small divit in the center of the shaft. I ran the tailstock up to it and the tip of the tailstock fits right into that divit, it couldn't get any straighter if i tried.

I took my heavy welders gloves and grabbed the bit and wiggled and pulled and the bit never moved so its not loose. If it had been loose it would have caught on the side of the wood it was cutting seeing as it was cutting about 3/4" at the time, that never happened.

I tried pulling down on the Z while the motors were engaged, even when it was almost to its bottomingout point and it never moved.

I centered the wood good before starting and it was spinning good. I wanted to make sure of that.

Here is the code that the indexer virtual tool wrote that corresponds to the second interface picture:
VD,,5
'----------------------------------------------------------------
SA 'Set program to absolute coordinate mode
SO,1,1 'Turn on router
PAUSE 2 'Give router time to reach cutting rpm

' file cuts in 1 rough passes plus a finish pass
ZB
MZ, 1.5
MX,0
M5,0,,0.9375,,360
MB,720
ZB
M5,32,, 0.9375,, 576000
ZB
MB,360
ZB
MZ,1
MX, 0
MZ,0.9375
M5,32,, 0.9375,, 1152000
MZ,1.1875
SO,1,0 'Turn off router
END

It was only supposed to take 1/8" total. Do you see anything wrong? If you notice the bit stepdown was only set to .1250 and you can see in the picture it took .50 in one big bite.

I am going to try it again, maybe it was just a fluke. The piece i rounded prior to this turned out fine.

Maybe i'm wrong but it seems to me that for operations like rounding and tapering it would be simpler to be able to zero at stock surface, then tell it how far down you want to go, then how far. That is how it is done manually on the Legacy and that works fine.
Let me know if you see something wrong in the code. thanks

[cmagro]

Code is correct as far as not tapering...

Slightly off your subject here...

looking at the rotation numbers the rough pass rotates 1600 times (576000 / 360) and the finish pass rotates 3200 times... Using an est. one second per rotation am I correct in saying it takes about 1 1/2 hours to round a square section 32" length....and that's just one step down??

Is this correct??

I don't understand the depth of the rough being the same as the depth of the finish...like Cut3D the purpose of the rough is just to remove enough material so the finish bit (which is usually smaller and more delicate) can handle the remaining material.

And to simply round a blank....for an inch square blank and only wanting to remove 1/8"....I would use a 1/4" spiral and run it back and forth along the length...rotating the blank two degrees (5 degrees might work great too) each pass.

Using..say...3" per second it would take 10 seconds per pass at 180 passes (360 / 2 degree increments). Finished in a half hour at worst case. This task should really only take about 10-15 minutes. And as a bonus you are cutting with the grain instead of against the grain..with the hardwoods I use doing it this way requires almost no sanding.

Tell you what....as you practice on the indexer send me info on what you are doing (i.e. blank size, length, task etc.). You do it your way and I'll use a method I like to call "the right way".

HA....had to throw that in...just watched the movie RocketMan with my little boy (very funny flik).

We'll compare ideas....share info....and people like Dana will get excited and buy an indexer. Shopbot will be so happy I will receive a surprise package in the mail (a 4HP spindle).

If you want you can post info or just email me...

Christian

[bill.young]

John,

There's nothing in the file that would cause it to cut a taper like that, so I'm guessing that Wayne is on the right track...that you've lost Z-position somewhere. Did you check to see if the tip of the bit was still at the correct zero position after it cut the taper?

Bill

[jdgrahamwaldorf]

I had a problem last year with the indexer virtual tool where I was turning a round blank that mysteriously tapered. I could watch the steps actually change on the screen when they should not have moved. I then ran the piece with the start radius and finish radius off by 0.0001 and got my correct turning. I thought this was fixed in the recent releases but I have not had a reason to check it.

John

[bill.young]

Hi John G,

If I remember correctly that was fixed in the transition between the 3.4 software and 3.5, but I must admit to being worried that your problem had crept back into the software somehow when John H. posted about the taper! I ran his file in the most recent versions of the software, though, including the 3.5.10 beta which I believe he said he was running a while back, and they all checked out fine.

This is a good time to remind everyone to make sure you keep your control software up to date, so that you have all the current bug fixes and newest features. And if you find something that you think is a bug, please send us an email about it so that we can work on getting it fixed.

Bill

[myxpykalix]

Christian,

I didn't answer some of your questions above so i'll do it now.
"looking at the rotation numbers the rough pass rotates 1600 times (576000 / 360) and the finish pass rotates 3200 times... Using an est. one second per rotation am I correct in saying it takes about 1 1/2 hours to round a square section 32" length....and that's just one step down??"

No, although I don't recall specifically the time frame to round the 32" was in the 10-15 minute range.

"and that's just one step down??"

even though the TOTAL stepdown was 1/16th of inch (for a total of 1/8th inch)and in the wizard I allowed a .1250 stepdown maybe i should put the stepdown value the same as the depth value?
Either way as you can see it took .50 off (a .25 depth).

[bill.young]

Hey guys,

The reason that the rotation numbers are so high in John's file is that he has the stepover value set at .01", so that it only moves that far down the blank for each revolution. If you're using a small ballnose bit then that's probably a good value to get a smooth surface, but if you're using a larger ballnose or maybe a 1/4" straight bit then you might be able to bump that up to .1" or so to speed the file up.

As usual it's a toss-up between speed and cut quality.

Bill

[myxpykalix]

I don't know if this matters as to it cutting tapers but I have been using a 1/2" staraight cutting endmill and the cutting time I thought was not unreasonable. Given the big bites it was taking I think it would have caused a problem using a 1/4" bit. The cut quality was smooth as glass.