Lathe question.

[chopsley]

I've programmed lathes for years but not with Mastercam. Say I want to face a part to centerline to take care of the saw cut with a CNMG style insert. I then want to go right into roughing out the OD profile with the same tool without sending the tool home. I'm sure there must be a simple answer to this. Thanks for any help.

[ReDEyZZ]

You can set a retract for each tool in the toolpath parameters page, where it says "home position" select "define" and you can set it there.

[chopsley]

Thanks Jarrett! I'll try that.

[Colin Gilchrist]

In Mastercam when you are programming Lathe operations with the same tool, it will just keep using that tool without doing a toolchange (depending of course on your post).

 

So in the ops manager, you would start with a facing toolpath, then create a Lathe Rough Toolpath using the same tool. You can create any number of toolpaths using the same tool, and Mastercam shouldn't put in a home move or a toolchange.

 

The thing you need to be extra careful about in Lathe is when you do change a tool. My number one suggestion is to learn to use the "Reference" points. This allows you to put in an "approach" point and a "retract" point for each toolpath.

 

Use the Ref points to bring your tool to a safe position before the tool approaches the workpiece, or a safe position before the tool moves home for a toolchange...

 

HTH,

[chopsley]

Thanks Colin,

 

I've heard about the benifits of reference points. From what I understand you just include them at the beggining and end of the chain. Especially with ID tools. Right? I'll experiment with this but I appriciate the help in getting me on the right track.

 

[FP1]

I don't know what all the fuss is about reference points on the lathe side. I have done a couple hundred programs between X2 and X3 and only needed reference points twice. In both cases it was a boring bar making a rapid move, through the part to the tool change position, directly from the back of the bore. I never could figure out what was causing it. It was clearly visible in back plot so I used reference points to pull out first.

[Colin Gilchrist]

Yes, that is basically right.

 

For example, say you were doing an internal groove inside a bore you had already cut and you had several grooves to do.

 

You would put an "Approach" reference point on the first groove toolpath. The tool will go to this point first, then move to the start of your "lead in" for the toolpath. The cutter cuts the groove shape, then retracts using your "lead out" and also possibly your stock clearance value.

 

At this point you are still in the bore and you need to do more work with this tool. You don't want a "retract" point on the first toolpath because you aren't done using it. The only exception would be if you had some shoulder or other geometry you needed to clear.

 

So for your next toolpath you would create a normal groove toolpath with no reference points. It will move from the end of the first groove path to the start of your 2nd path at rapid.

 

Now you create your third groove toolpath, this time you would use only the "Retract" reference point to get the tool to a safe clearance point before it goes home to change the tool.

 

Make any sense? It is really easy once you get the hang of it.

 

I'd advise you to put in some "home position" values and turn on the "show lathe home position" option in backplot.

 

That way you can see if a tool is trying to rapid through your part on the way to a toolchange.

 

I find that I do much more backplotting in Lathe and less verify. Since it is mostly 2D, it is pretty straight forward...

 

HTH,

[Colin Gilchrist]

FP1,

 

For the most part you are correct, especially when doing mostly OD work. The problem is that one time when you do need it and forgot to use it.

 

Let's just say I've only made that mistake one time...

 

You just don't forget noises like that...

 

:-D

[Bob Hedrick]

Here is a rule to follow to avoid crashes for ID work without reference points:

If you are using a ID tool, the holder should be long enough so that it sticks out beyond the face of the part (normally +Z) when the tool is at its most negative Z coordinate. This helps the software decide which way to retract from the cavity. If this isn't practical, then reference points are the way to go.

[Mike S @ S4A]

nobody's appears to have addressed stock definition in this thread...most important IMO for ID; that's how mcam knows where it's safe to retract

[generaldisarray]

+1 to Mike

 

That is one of the first things I do when creating a new program.

[Mike S @ S4A]

Thanks Gen'l....

didn't say so cuz I'm smart, said so 'cos of the dozens of tech support calls JP and I have taken on this very issue....

[Chris Rizzo]

Ahhh,

 

So it's the holder. Any other toolpaths where holder definitions are critical? Cut off maybe?

[Colin Gilchrist]

Interesting...

 

I'll have to try this with a couple of toolpaths.

 

Thanks for the Tip Bob!

[Bob Hedrick]

Chris,

The holder is collision checked on ALL turning operations, if you've defined stock. Currently one boundary is wrapped around the insert and holder, which means the software won't generally catch a feed move that embeds the holder into your stock.

 

Colin,

Good luck with the testing!

Let me know how you make out.

 

One more thing...

For collision checking to work properly, make sure you have 'Write home position clearance moves' checked on the Machine Group Properties Tool Settings page!