Lathe Threading tool parameters

[Greg_J]

Hey Guys,

 

In the threading tool parameters tab at the bottom the compensation setting is greyed out, MC help file says that it's unavailable for threading tools.

 

If you look a how its set, it's set to center.

 

Who touches off their tool that way?

 

Usually it's touched off from the front of the tool and the tip, every probe I've seen works this way.

 

So we program the thread with the tool set to the default operator touches of the front and the tip, so the simulation in MC is not the same as what happening at the machine.

 

We have to clip all our threads so I do this in MC the clip doesn't work out correct cause the tool was not set up to how MC has done it.

 

Question #1

 

Is there a way to ungrey that field or get MC to use the front of the tool not the center? I can't create a custom tool for threading it still greys out that field I want to change.

 

 

Question #2

 

Another issue is that you can only use threading tools to thread, we use a grooving to in a threading cycle to thread clip, so is the only way to do this in MC is to create a custome tool and thread with that?

 

 

 

The only way that I can see to get it to work is to call all my threading tools a grooving tool so I can adjust the compensation setting.

 

TIA

 

Greg

[Colin Gilchrist]

Hi Greg,

 

Since there are no Cutter Compensation codes output for a canned threading cycle, we don't support the compensation options for threading tools. You can get around this by creating a Custom Tool definition, and drawing your threading tool as you would touch it off in the machine. Just draw the tool so that the front edge of the tool/holder is on the Y axis, and the tip of the insert is tangent to the X axis. (In Top view). Draw both the insert shape and the holder shape as two closed boundaries. Make sure you use either Color #14 (insert up) or Color #138 (insert down), and draw the holder boundary in Color #116.

 

When I draw a custom Lathe threading tool this way, there is a 'Geometry' tab in the tool definition dialog box. You need to pick a level, or draw the tool geometry in a separate MCX-6 file. There is an button for 'Tool Center' that you can use to pick the compensation point (the point you touch off too on your machine tool). If you've drawn the tool properly, you should be able to click the button for 'Tool Center' and then pick the system origin for the tool center point. This will cause the cutter to compensate properly, and make Backplot match the setup on your machine.

 

Here is a picture of the custom tool geometry I drew:

 

 

Notice that I drew the tool with the leading edge on the Y axis, and the tip of the insert on the X axis.

 

Here are the lathe thread shape parameters:

 

 

Notice that the End position of the thread is -20 mm, and the thread depth is 2.2 mm. (1.1 mm radial depth).

 

Here is a picture of Backplot showing the Custom Lathe threading tool. The lines show the correct positions: -20mm in Z, and 1.1 mm thread depth:

http://i93.photobucket.com/albums/l66/colingilchrist/CustomThreadToolFinalPass.png

 

 

Now here is a screen shot of a standard lathe threading tool, with the same thread parameters. All I did was change from the custom lathe tool to a standard lathe tool:

 

 

 

I hope that helps on creating the correct threading tool.

 

Can you provide more information about the 'Thread Clipping'? I'm not familiar with that term for Lathe threading and I'm curious as to what you are doing with the tool? With some more information I can help you come up with a solution.

 

Thanks and best regards,

 

Colin

[Greg_J]

Thanks for the info on the tools.

 

I have many many different threading tools so I will have to create a tool for each one, one way that I found and would save me a lot of time is when I have the tool definition open I can click the button on the top right that says draw tool. If I can have access to those drawings. I could just copy them and reposition them, but I can select the drawing and copy but when I paste them there's nothing there.

 

Regarding thread clipping.

 

For example when you cut a 4 full acme thread and where the thread enters and exits the part it tapers down to a very sharp edge. We remove that sharp edge with a grooving tool. We use a threading cycle and just thread deep enough to remove the sharp edge of the thread usually about half the pitch deep and we cut to the major or minor depending on internal or external. On external threads we clip front and back on internal we usally just clip the front and deburr the back by hand.

 

I'll post some picutres in a bit.

[Colin Gilchrist]

Greg,

 

 

To save the geometry from an existing Lathe tool, start by opening up the Lathe Tool Manager. Select the tool you want to get the geometry for, and right-click. In the pop-up menu there is an option to 'Save geometry to file' and 'Save geometry to level'. So you can do either one.

 

You can also select a Lathe Grooving Tool for use in a Lathe Thread toolpath, but you still won't be able to Comp the tool in Mastercam. You'll have to measure the zero point of the threading tool, and adjust the zero point of the grooving tool in the Control to get the position correct.

 

I looked up the thread clipping, and this is also referred to as a 'higbee thread cut cycle'. (although a true higbee eliminates the first thread completely, and tapers the 2nd full thread)

 

Hope that helps,

 

Colin

[Greg_J]

Thanks for the help Colin.

 

I have another question for you.

 

Is there a way in MC so set the starting spindle orientation on a threading cycle.

 

G76X4.457Z-2.3Q0K.144D.03I0.F.5

G76X4.457Z-2.3Q18000K.144D.03I0.F.5

 

The above code is a double start 4 full acme.

 

I was able to get MC to post out the correct Q value but some times when it comes to thread clipping I would like to play with the Q value to make the clip come out correct.

 

I do this with threadmilling, I am able to clip the thread and I play with the start angle to make it perfect.

 

Is there a setting that I can use to adjust the start angle in the threading cycle?

 

Thanks again!