lathe ID grooving

[Chris Rizzo]

Cutting an ID groove, and mastercam seems to be driving the centerline of the tool on the centerline of my chained geometry, thus the groove to too wide by the width of my cutter. Just like in mill if cutter comp is turned off. I'm probably missing something simple..

 

thx

[crazy^millman]

Make sure you have your tool defined right on the set-up. If you sre using back and the set-up on front then you will see this exact thing.

 

HTh

[Rakesh]

Chris,

Never have the problem. Give little more inf, your problem will be sought out easily.

[Rakesh]

One thing I can quickly think of, on groove finish parameter,there is compensation type in your case it look like it is off and it should be on computer,

[Chris Rizzo]

 

 

 

 

The brown line in the first photo is my driving chain. The dotted line is what's getting machined. In the 2nd photo you can see the tool violating the driving geo.

 

I'm using a custom defined tool, which is drawn on level 100.

 

thx

[RObert TImby]

Check your cutter comp it should be on computer or wear. It be on off

[Chris Rizzo]

Comp is on computer. The other weird thing is that on right side of the groove boundry, the tool overcuts slightly more than on the left side. Maybe I should save as geo and see exactly what it's doing on either side..........

[gcode]

Chris, If you want to upload your file or email

it to me I'll take a look at it.

[RObert TImby]

Can you e-mail it and i will take a look

[DavidB]

Use tools width in Plunge cut parameters

[dwsz71]

I've had this happen when taking in a library tool, modifing the insert parameters without saving the new "job" tool back to the library as something different than the original. It would reference the library tool instead of the "job" tool when creating the toolpath.

[Mike-T]

It looks like a custom tool, you might check your lathe tool clearance on the tool parameters page.

[Chris Rizzo]

Thx fellas. I just parked it on the FTP, it's under MCX2, file is PLUG.MCX.

[Hymen]

You don't have your tool defined properly!!

[Hymen]

follow these

edit tool

param tab

tool clearance button

define width and depth

 

since there is no radius on the tool for now pretend there is and call it .002. you will do this so you can have a graphical representation of the things you just defined. Keep in mind that they will not appear exactly tang to the tool lines but will be off by half the radius you defined . Unless of course you defined the center of the radius with the button that is below the rad box. When yur done set radius back to zero.

[Hymen]

You need to fix the direction of it as well

 

I really like photo bucket!!!

 

these you have to play with a bit to get the hang of how it's used. Read the orientation notes.

[Chris Rizzo]

Thank you all for the assistance and good pics. VERY much appreciated for this lathe rookie.

 

 

If I do spec a corner radius, then it looks like it once again machines outside the boundry. Would it just be better to draw the radii on the custom tool anyway, and leaving the value at 0?

[Rakesh]

chris

Did the grooving working right for you now?

I tried your file and with little modifications it is working right now.

[Hymen]

Chris,

The only reason I asked you to add a radius was for a visual to ensure you had the tool defined properly. If you do not specify a radius then you don't get a visual. So after you've defined the tool and it looks ok visually then you need to remove the radius and reset the center of tool to zero if you've changed it. If the tool has no radius then no don't draw the radius and vise versa. All three circles will be inside the tool if it has been defined properly.