wire - taper angle exceed limits

[klemen]

I would like to cut a simple wire contour (click), but i receive a "Tapper angle exceed limits set in machine definition." error. Why is that? What machine definition is this?

 

I use the default machine type.

[Steve Biehl - Cimquest Inc]

can you put the file up on the ftp site so we can take a look at it?

[Guest]

Can you send a z2g file so I can get a look at what you're doing and your setup

[Thad]

klemen,

 

I'm not a wire guy, but if you go to Settings-Machine definitions (I think it's under Settings) and look through the parameters of the Generic Wire EDM machine definition, you'll probably find a setting that states the maximum taper angle. It's probably set to less than what you're trying to cut.

 

I'm sure the actual machine has a limit on taper angle so you should set it to your machine specs.

 

Thad

[Guest]

klemen, if you are using 4 axis, then make sure you are using sync either by entity or branch.

[Roger Martin from CNC Software]

Maximum Taper Angle is a physical machine limit, so that setting is in the Machine Definition (not the Control Definition).

 

From the Mastercam main menu select ->

Settings.

Machine Definition Manager.

Open your Wire Machine Def (WMD file).

Click on the ‘General Machine Parameters’ icon in the toolbar.

On the ‘Op. feed rate limits, axis motion’ tab page you’ll find the Maximum wire taper angle setting.

 

Also as Del points out ->

Make sure that you are sync'ing properly.

 

Also, this is just an FYI warning message.

In the end, if you know that you're OK with what you are programming, you can post it out.

*Mastercam makes no NC code changes because of this warning message.

[Jerry_P]

I keep getting this message when I try to use Wire Path Point. I am not cutting taper, and the taper is set to 30 degrees in the .wmd file, which is maximum for the machine. I do not get it any other time, just when I try to use point. Am I still missing a setting some where or is it a minor bug with the new patch. And like you said it still post just fine. It is just annoying as heck because every time I open that file that error pops up for each Wire Path Point I have in the file.

[edmBosto]

Jerry,

I'm not at work but what is the machine definition x,y,z set to? If the Z is 10. try setting it to 0 and see if that helps.

[edmBosto]

I believe the Machine def. start point is set to 10 inches on the Z for milling purposes.

 

I have my Z set to zero.

quote:

---

What machine definition is this?

---

Go to

Settings/

Machine Def. Manager/

In the lower right Machine Config. window in machine Base, under Upper Wre Guide Group, double click on the Z Axis icon and a new window will open for the z axis. Change Initial Position to zero.

Then save the settings and then replace your machine in the tool path manager under properties.

 

HTH.

[Jerry_P]

Yes I think that did it thanks

[edmBosto]

Steve Biehl taught me that awhile ago on one of his visits.