LATHE TOOL OFFSET

[SBA]

I was wondering if anyone has found that the

tool offset for setting to tip in x and center in z, does not set as shown. Sets at center/center, or am I missing something?

[Chips Ahoy]

SBA

Is it on all turning tools? Are you using radius compensation? Turn it off. Which ever you want. I prefer radius comp. during finish turning and boring only. Sometimes I use it during finish grooving also. Then you can comp. at the control. One way around this could be to make the tool sharp with no radius. But, I am not sure of your exact problem though. Need more info. Rick

[SBA]

The problem is using cutter comp. and selecting to compensate from tip in x and center in z. It is a boring bar operation under cutting an inside diameter, the tool is a vnmg style insert in 27 degree 30 minute lead style bar. The center of the insert radius is given from the end of the boring bar. We set the tool offset in the control from tip in x and center in z. When programing using tip x and center z offset on the tool is sets it at center in x and z. There is a selection for center both and a selection for tip and center, but they seem to do the same thing.

[sbrooks]

SBA

Go in to the edit page for that tool.The last tab is parameters,on the bottom left there is a selection for different points

on the tool that you can make zero.

[gstephens]

SBA sent me the file and I stripped out the non-pertinent info and posted it to the FTP site.

Mastercam Forummc8 files130571-A.MC8

The Center/tip offset seems to be offsetting Z instead of X in this instance. T11 is Center of Radius, T13 is Center/tip. Backplot them with tool and toolpath on, but with verify off, and you'll see what I mean.

I think the tool may need an orientation change, but I can't figure out how to get it right.

Ideas anyone?

[ 09-25-2001: Message edited by: gstephens ]

[Chips Ahoy]

Is it maybe reading the wrong quadrant for the tool? With radius comp we would use quadrant #2. Don't know if this will help???

[gstephens]

OK. I found out that you MUST create a custom tool with the origin at the offset position for this to work. My suggestion is to build the tool as normal (with insert and holder) then draw the tool and save the geometry. Open up the tool .mc8 file and move it to the correct origin position. Then define the custom tool in the library with the appropriate settings and your set.

SBA - if you need more info, let me know as I have the tool created and the toolpath run already.

[SBA]

The problem as best I can see is fixed best, as recomended above, by creating a custom tool, setting it at tip/center and selecting same on parameter page. Most tools work just fine without any problem, there is something different about this one.

Thanks

[gstephens]

A request has been logged with CNC. Apparently the orientation of a default bore-bar is such that the Z tangency of the radius is what is assumed instead of the X tangency, and you can't adjust the orientation on a standard (insert-holder) tool.