On lathe with c axis face contour can you force x axis to the positive side?

[Leon82]

The live tool can't reach on the lower face and it's not posting a rotation. (2 chains in one op).

Can you make it rotate to c180 for the second chain?

[Alex Dales]

With Y-axis cutting? I think you will have you use a second op and twist the tool plane by 180 degrees to indicate the C180 to the post.

[Leon82]

6 minutes ago, Alex Dales said:

With Y-axis cutting? I think you will have you use a second op and twist the tool plane by 180 degrees to indicate the C180 to the post.

No y. Only c.

 

If the guy uses two ops it runs both on the plus side.i think we will check now

[crazy^millman]

Toolpath transform rotate the 1st operation if they are exactly 180 from each other.

[Leon82]

Even with transform it does the same .

[Leon82]

I put a call in with the dealer. They say it was working before.

[crazy^millman]

1 hour ago, Leon82 said:

Even with transform it does the same .

No the one chain would have to be picked that is in the correct place. That operation would then need to be rotated. If the Chain is spread in such a way that trying to machine it in one operation is not possible then you have to make it one operation and transform rotate that operation to get the feature 180 from there. It also comes down to where and how you defined the operation and the planes to drive it. I did a sample file with MPfan and got the results I would expect to see. Have you tried using a Generic Post to see if it works?

[Leon82]

39 minutes ago, crazy^millman said:

No the one chain would have to be picked that is in the correct place. That operation would then need to be rotated. If the Chain is spread in such a way that trying to machine it in one operation is not possible then you have to make it one operation and transform rotate that operation to get the feature 180 from there. It also comes down to where and how you defined the operation and the planes to drive it. I did a sample file with MPfan and got the results I would expect to see. Have you tried using a Generic Post to see if it works?

I used the default lathe and it was the same. If I do a plain milling face contour it is correct. He may not have the plane correct. we sent a ziptogo off.

[Alex Dales]

Hmm with a C-axis rotary style is seems very strange that your face milling is giving a negative X value at all. 

mplmaster calculates the C axis as follows:

          if abs(cuttype) = 2,
            [
            if fmtrnd(xa) = fmtrnd(prv_xa) & fmtrnd(ya) = fmtrnd(prv_ya), csav = prv_csav
            else, csav = atan2(ya, xa) + c$   #on the face you need to add c$ in case of twisted face plane
            ]

ya and xa are the rectangular coordinate on the face, so if your rectangles are 180 degrees apart, then the calculation should also be 180 off.

I would try commenting out the c$ and see if that makes any difference.

[crazy^millman]

I guess the question comes down to is he using the C axis toolpaths in the Lathe or the Milling toolpaths and then coming back and changing them to C axis toolpaths. There are different ways to go about it and each one presents their own method to get correct NC Code.

[Leon82]

It's using g112 and if keep tool down is not selected it keeps turning it on and off. All the other programs seem to turn it on at the beginning and off at the end. At some point the post-processor was updated.

 

But something like a hex it works perfectly fine. 

We're going to do an experiment tomorrow and then we'll have to see if they can modify it.  

1 hour ago, Alex Dales said:

Hmm with a C-axis rotary style is seems very strange that your face milling is giving a negative X value at all. 

mplmaster calculates the C axis as follows:

          if abs(cuttype) = 2,
            [
            if fmtrnd(xa) = fmtrnd(prv_xa) & fmtrnd(ya) = fmtrnd(prv_ya), csav = prv_csav
            else, csav = atan2(ya, xa) + c$   #on the face you need to add c$ in case of twisted face plane
            ]

ya and xa are the rectangular coordinate on the face, so if your rectangles are 180 degrees apart, then the calculation should also be 180 off.

I would try commenting out the c$ and see if that makes any difference.

I'll see if I can get my boss to download a shot too

[Alex Dales]

I have never seen G112 act like that and try to cross X0. Maybe it has something to do with the start/end points of the two passes and the machine is trying to avoid doing some sort of large rotation near X0. Could be a machine parameter, but nothing I have run into before.

Are you able to upload the code? Maybe there's something I'm missing.

[Alex Dales]

The on/off on the G112 does seem odd though. Is the C at 0 when G112 is being re-enabled? If there is already a C value when its activated then it can re-set the zero and act like a twist.

Try calling a C0 before the second G112. That seems like the most likely fix to me.

[Leon82]

Yeah there's something weird going on with it because the description for miscellaneous integer for has disappeared. This is the switch for g112.

After he handed the code turning it on and off only at the beginning and end it seemed to work good.

I wonder if somebody inadvertently overwrote something

[crazy^millman]

2 hours ago, Leon82 said:

Yeah there's something weird going on with it because the description for miscellaneous integer for has disappeared. This is the switch for g112.

After he handed the code turning it on and off only at the beginning and end it seemed to work good.

I wonder if somebody inadvertently overwrote something

Could be a permissions issue with the LMD and Post that Windows messed up.