5 Axis y Axis Linear Limits

[KBHokie]

I'm having a problem with the NC code for our 5-axis machine.  The issue is the spindle can only reach half the table so all y values have to remain positive. 

I can't figure out how to fix this.  Is it something in the post, the machine definition, or tool path?

I've done the following to try and alleviate this issue:

  -Changed the y-limits in the machine definition

  -Changed the y-limits inside the post. 

Does anyone have any suggestions?

Thanks for the help!

 

[Watcher]

You just tripped over a complex subject... 

[crazy^millman]

You must program with this limit in mind. The post cannot fix kinematic limitations. It can warn you or stop posting when it runs into them, but you must break up your operations to not over travel in the Y axis.

[KBHokie]

Thanks for the response.

I'll break up the tool path accordingly.

Is there an easy way to set the C axis while doing a 5 axis drill tool path?

[mkd]

1 minute ago, KBHokie said:

Thanks for the response.

I'll break up the tool path accordingly.

Is there an easy way to set the C axis while doing a 5 axis drill tool path?

Toolplanes. one hole at a time.

[KBHokie]

I can't seem to get the part to rotate 180 degrees using the tool planes.    All of the holes are on the top of the part so ideally I would want to drill all the holes on one half then rotate the part 180 degrees then drill all the holes on the other half. 

Any suggestions on how to do this?

[Guess_who]

This has been a complaint of mine for some time. He's some ideas you could try;

try to do a dummy move close to your position, like if you're trying to go to say A0 C180, and it keeps posting A0 C0, do a dummy move at A0.5 C180 drill air, then go to A0 C180. - This used to work, not sure if it still does.

Also, I've accomplished this by slightly moving off A0. (or whatever is perpendicular to spindle), if you have the tolerance, try to go to A0.001 -  Basically, whenever the spindle is perpendicular,  Mastercam thinks the rotary can be anywhere and it doesn't matter.  But if you move the table just slightly it is forced.

[crazy^millman]

Can't get the part to Rotate? Sorry can you explain this a little better? You are duplicating your top plane and then editing it 180 degree. You are then using it as your C-T Plane for the operation you are trying to get rotate. I have done this many time, but it can be some work getting it all sorted out and going in the correct direction.

[KBHokie]

Thanks for the quick response.

Yeah, that's exactly what I did.  I took my top plane then rotated it about the z-axis 180 degrees.  I then used this for my Tool and Construction planes, and I left my WCS plane the as the original top plane.  I'll play around with it more tomorrow.   

Does it have anything to do with the origin being in the center of my part?

[Leon82]

If you don't mind doing it by hand you can simply put c and y values in the drill cycle. You can manual entry an entire program file (your rotary drill program) so it will post somewhat clean.

 

I have gotten mine do drill with x and c with 3 axis toolpath in rotary tabs, rotation about z.

I was playing with the machine def at the time so I have it as a 4 axis not using A on the trunion. This was for one off stuff, we use camplete for everything.

I had the same issue but want to post x negative. 

 

 

[Guess_who]

Also, in my post I have the below option in my misc variables which help to position. Doesn't alway work, but I just did a test and it successfully posted to A0 C180. When this was set to 0, it posted A0 C0 regardless of my plane being rotated 180. You may look and see if you have something similar.

 

 

[huskermcdoogle]

If you do as Ray D has mentioned in previous post, select force tool change and it will probably work.  That's what I had to do to get mine to work.  Not sure if that is something that can be changed in post to respect the misc int at a null tool change.

Also remember that if you change misc ints/reals you need to regen even though they don't go dirty.

[huskermcdoogle]

2 minutes ago, huskermcdoogle said:

Not sure if that is something that can be changed in post to respect the misc int at a null tool change.

Look for the following in your post.

bias_null    : 1     #mi4 and mi5 bias are applied at null toolchanges

Set to 1 and it should work without setting force tool change.  Also, now if you do change this, understand that posting any new programs forward with this post will result in potentially different behavior.

 

[Guess_who]

3 minutes ago, huskermcdoogle said:

Look for the following in your post.

bias_null    : 1     #mi4 and mi5 bias are applied at null toolchanges

Set to 1 and it should work without setting force tool change.  Also, now if you do change this, understand that posting any new programs forward with this post will result in potentially different behavior.

 

 

I just checked mine and it is also set to -   bias_null   : 1   as Husker suggested.

[Mick]

Force toolchange is one of my most commonly used functions in Mastercam for 5 axis work. It has got me round issues like this a number of times.

[Grievous]

What machine with what controller you have?

[KBHokie]

Thanks guys the forced tool change idea worked, along with changing bias_null: 1in the post.