Indexer tool refresher needed?

[myxpykalix]

I usually use a app i wrote for spirals and turning round but it is on a HD that won't let me access it at the moment so i need to use the indexer tool within the control software to turn a square to a round and i need some refresher questions answered since i haven't used it in a long time.

Under Tools/Indexer I go to
Turn a blank to a finished size
Turning settings
Rough blank radius 2" (it is 2"x2")
finish radius at start point of turning pattern= 1.5"
finish radius at end point of turning pattern= 1.5" I want it to be 1.5" all . the way down
I know the rest of settings
I guess my question is, i don't recall, Do i set the Zzero at the tip of the diamond shape of the material (the sharp edge, highest point in the turning) or at the flat of the material?
My memory is getting worse and worse...

[Brady Watson]

Under Tools/Indexer I go to
Turn a blank to a finished size
Turning settings
Rough blank radius 2" (it is 2"x2")
finish radius at start point of turning pattern= 1.5"
finish radius at end point of turning pattern= 1.5" I want it to be 1.5" all . the way down
I know the rest of settings
I guess my question is, i don't recall, Do i set the Zzero at the tip of the diamond shape of the material (the sharp edge, highest point in the turning) or at the flat of the material?

Dude...I thought you were the indexer EXPERT!

You nearly always set the Zzero at the CENTER of the blank. This way all measurements will be from the center outward, which is what you want. You would only want to zero to the top if you were doing a shallow engraving or were doing a 2 or 4 sided 3-axis toolpath using the indexer to swap sides. Using the Zzero plate on top of the material is awkward at best & will result in a false reading unless the blank is absolutely level (and the plate is level), which is dicey at best...this is another reason you zero to the center. I pretty much ALWAYS zero to the center of the indexer...which means that your material Zzero is referenced to the "bed/table" and NOT to the top of the block.

If you want to make life easy, put a piece of masking tape (as an electrical insulator) on top of the flat of the tailstock. Then, use the Zzero plate on top of the masking tape. Then lower the Z down until the bottom of your bit is at the exact height of the live center point in the tailstock. Write down that value on the masking tape you just put down. Now you can easily zero tools reliably to the top of the tailstock, then use the VA command to assign the current location of the Z (read what the DRO says) PLUS the number you wrote down as the distance from the top of the tailstock to the live center point. This number will be POSITIVE. So if after running C2, it parks the Z at 0.5" above the tailstock, and let's say it is 1.524" from the top of the tailstock to the live center point, then you would call up the VA command and enter a POSITIVE value for the Z axis of 0.5 + 1.524 = 2.024 ~ Now your tool will be zeroed to the center of the indexer reliably. If you really want to hook yourself up, make a custom cut that when run just uses the VA command to assign the Z axis to 2.024 when you run it...

The indexer tool specifies rough blank radius NOT diameter...So keep that in mind when you program values for the Z. This is true for other values in the tool. You always have to be aware whether you are running in radius or diameter "mode" when you program and set things up. It can get you in trouble if you are asleep at the wheel. You have spec'd out 4" diameter material...not 2" diameter/1" radius material in your post above. You'll also want to consider the additional material the corners add (by multiplying one of the 2" sides by the square root of 2, and then divide by 2 to get your actual max radius...If you don't, the corners will most likely blow out and shoot across the room:

2X2 material:

2" X √2 / 2

2 X (1.414) = 2.828" (Diagonal to diagonal of 2" square stock)

Divide by 2 to get RADIUS: 2.282 / 2 = 1.414" MAX RADIUS @ Corners

Hopefully that gets you going...Have a cup of coffee & try to understand it...You might have a breakthrough...or a breakdown!

-B

[myxpykalix]

Because i had not used the indexer tools within Control panel for years i have gotten confused.

The app i had been using was written so i could simply Zero to the material surface, insert the depth i want to go (based on the bit and profile) and basically hit the start button and go.

I was confused on the diameter/radius terminology
My app used diameter for input references

What i usually do is run the router down to cut off the sharp corners because in the past i have done exactly what you described of burying the bit.

I recall having a jig to measure Zzero-center of material (just a precisely cut 2x4)
So i'm starting to recall the steps and the the only thing i have to be aware of is a 2"x2" square has a 1" radius to get to center.

I'm sorry i couldn't remember those steps and got confused but you need to remember i'm not a Young Whippersnapper like you!

I appreciate your detailed answer and i will digest it more thoroughly but think my confusion was the radius/diameter whatchamajigger