X9 Lathe tool clearance on Finish Groove

[JeremyV]

I'm using the finish groove option to finish a face groove tool path.  After the 2nd plunge, the tool rapids out to Z 0.0 instead of Z.1.... that simply won't do since the machine homes towards X first then Z.

 

I also noticed the other tools - finish face only clears the face by .03 ... I was wondering if you can control the clearance of the tools... cause I don't want to scare anyone lol...

 

 

-JD

[Colin Gilchrist]

The rapid clearance is set in the "Tool settings" of the Machine group properties.

 

When in doubt, always use Reference Points, to give an "initial" approach point, and a "final" retract point...

[JeremyV]

Well.... the .1 clearance works for everything else except the finish groove option cause i am following the chain.   I really don't know what i am doing wrong.   Even changing the "tool settings" does not affect the finish groove exit point.

 

The rough groove works the way it should when following the chain.

 

I also have no options for exit point as well.

[Parrish80]

For all id toolpaths, and face groove toolpaths, I always always always use Z ref. points in the toolpath parameters for approach and retract.

[Colin Gilchrist]

Jeremy,

 

All Lathe Toolpaths have a "Reference Point" option. This is on the "tool" page. You have to enable the button itself. Then set  the options individually for start/end reference point.

 

I always, and I mean always use a Reference Point for all ID work. Turn on the check box, the button enables. The press the button and set your numbers in the dialog. It forces Mastercam to output an "initial point" move, and a "final point" move, and works 100% of the time.

 

Stated another way, if you don't use reference points for ID work, there is 100% chance that you will have a part/tool collision. It will happen. Reference Points are critical for ID work...

[JeremyV]

First... i'd like to apologize for sounding so frustrated.

 

I don't understand what you mean by "tool" page?  Do you mean when you click on the tool and right click on the tool to edit the tool?  In that area or somewhere else?  I know i'm new to Lathe programming and only got so far on my own and i've done surprisingly well, with exception to the groove programming.

 

So... can anyone show me a step by step directions on how to do this?

 

Thanks in advance if it's not too much of a bother.

 

Apologies again.

 

-JD

[Parrish80]

We've all been there, don't sweat it.

 

Open the parameters for your toolpath from the operation manager.

At the bottom of the window that pops up, it will say "ref. points" with a check box next to it.

check the box, a window will pop up, set your Z points in approach and retract to .1

make sure it's set to absolute, and leave the checkboxes for X unchecked.

 

HTH

[Colin Gilchrist]

Yes, no worries Jeremy. When you are on the First tab of a Tool Path Operation in the Dialog Box, there is a list of tools in the white space, upper left corner of the dialog box.

 

There are "tool settings" on the right, like "feed" in UPR (units per revolution) or UPM (units per minute), and spindle speed (CSS vs. RPM). Below these parameter fields are a series of check boxes. When you enable a check box, it "turns on" the button associated with the check box.

 

Reference Points is "grayed out" by default. So it looks like you can't use it, but you can. This button is above "canned text", and is just above the "green check mark", "Red X", and "?" buttons, in the lower right of the dialog.

 

1. Start by creating a new path, or selecting an existing one. If a new path, select your geometry.
2. This opens the toolpath dialog. Say you are using a "Face" path for your first path. It will open on the "Toolpath parameters" page. This is where you select your tool, and set speeds/feeds.
3. Above the "green check mark" and "red x" buttons, is "Canned Text". Directly above this is "Ref. Points", but the check box is "unchecked" by default.
4. Turn on the check box for Ref Points.
5. Now, press the "Ref Point" button.
6. In the Reference Point dialog, turn on the "Approach" and "Retract" check boxes.
7. Set the Diameter options (or don't). If you leave the box unchecked for "X" for example, it will use the starting/ending X point of the operation. This is "good".
8. So for our example, turn on only the "Z" option. Set the value to .100. Make sure both radio buttons are set to "Absolute".
9. Press the green check mark on the Reference Points dialog.
10. Finish entering the rest of your toolpath parameters.

You need to do those steps above on every single ID operation you create. Don't leave it to the "automatic" behavior in Mastercam, it will bite you eventually. Just get in the habit of using Ref Points for every ID OP, and you'll never crash a Boring Bar again...

[JeremyV]

Thanks guys.  I have X6 installed at home and I see what you are talking about.

 

I'll need to double check myself and see if those reference points checkbox was there in X9, cause I can't recall seeing it?

 

 

I'll let you guys know if i see it.    If that option isn't there.... i'm screwed?

[JeremyV]

Thanks guys, found it!

 

Works like a charm.... now to remember to select that lol

[[email protected]]

I'm using the finish groove option to finish a face groove tool path.  After the 2nd plunge, the tool rapids out to Z 0.0 instead of Z.1.... that simply won't do since the machine homes towards X first then Z.

 

I also noticed the other tools - finish face only clears the face by .03 ... I was wondering if you can control the clearance of the tools... cause I don't want to scare anyone lol...

 

 

-JD