5 Axis post- B & C axis unclamp

[Anonymous]

Hello- 

I am using post: Mazak vc 500 and I need to add a B axis unclamp M code (M46) and a C axis unclamp code (M43) in the post where the b and c axis is used at feedrate moves. 

Currently the b and c axis is clamped during 5 axis machining operations, which yields jerky movement.  

The machine control automatically re-clamps the B and C axis at the end of each program.  

Thank you for the help

[andrea.amilo]

Hello @Anonymous ,

I think the Mazak vc 500 post is already configured to manage clamp/unclamp functions.

You can find them commented in onCommand function.

The picture below shows you how I have defined these functions : 

Please test it carefully and let me know.

[Anonymous]

I see that.  

However I dont get any axis unclamp codes when I post.  None at all.  

I am currently manually entering them in the code.  

What do I need to do specifically to get it to post M46 / M43

Thank you

[andrea.amilo]

Hello @Anonymous ,

to have the unclamp codes I think you need just to :

- un-comment ( remove // ) lines 2737 and 2740 ;

- add 46 and 43 on the same lines inside existing command writeBlock(mFormat.format()) ;

as shown in my picture above (see message #2).

Please test it carefully let me know.

[Anonymous]

Ok I will try that. 

I am getting an error with C axis rewind.  

I have the post configured with c as a cyclic axis.  

Here is the error I get when posting:

Error: REWIND: Rewind of machine is required for simultaneous multi-axis toolpath and has been disabled.

Error at line: 2355

[Anonymous]

I made the edits you suggested BUT I still dont get the unclamp codes when I post a swarf operation.  

Here is what I have in the post.  

case COMMAND_LOCK_MULTI_AXIS:
if (machineConfiguration.isMultiAxisConfiguration() && (machineConfiguration.getNumberOfAxes() >= 4)) {
var _skipBlock = skipBlock;
writeBlock(mFormat.format(46)); // lock 4th-axis motion
if (machineConfiguration.getNumberOfAxes() == 5) {
skipBlock = _skipBlock;
writeBlock(mFormat.format(43)); // lock 5th-axis motion
}
}

[Anonymous]

Actually, it does post the unclamp codes BUT they are at the end of the program, not before the operation.

[andrea.amilo]

Hello @Anonymous ,

It seems you made the correct modification in the wrong place.

In fact you edited the    case COMMAND_LOCK_MULTI_AXIS:    as you wrote in message #6.

This part of code is related to the lock commands.

You need to make the same modification in   case COMMAND_UNLOCK_MULTI_AXIS:  as shown in my first reply, message #2.

Please test it carefully and let me know.

[Anonymous]

Ok do I  need to UNDO my first modification (in the wrong place)?

[Anonymous]

Nevermind on the last question....I am working to locate the lock M codes to insert in the lock section.

[Anonymous]

Problem here is that it unlocks the B and C axis on every operation....even when they dont need to be unlocked! 

[Anonymous]

@andrea.amilo - 

Problem here is that it unlocks the B and C axis on every operation....even when they dont need to be unlocked! 

Is there a fix for thix?

[andrea.amilo]

Hello @Anonymous ,

now you have the standard unclamp/clamp post configuration.

If you want to use unclamp/clamp only in 5 axis machining operations I think you can add :

&& currentSection.isMultiAxis()

in both the 'case' your a managing, as highlighted here ( lines 2725 and 2735 ) :

 Please test it carefully and let me know.

[Anonymous]

Thank you.

[Anonymous]

@andrea.amilo  I do appreciate the help. 

We are getting close to having this post worked out.  

Next issue is the B axis moves the wrong direction during positional moves.  It moves the correct direction during multi-axis machining moves (swarf).  

However, I we just want to use the axis for positioning only....B-90 for example, it moves B positive. 

I was working with Bob from autodesk late last week and he helped me fix the multi-axis contour moves and I didnt notice the positional move issue then otherwise I would have asked him to help. 

When doing positional moves, (2+3 machining) the b axis doesnt post as a B code but rather I,J,K.  

N19 G68.2 X0. Y0. Z0. I180. J90. K90.
N20 G53.1 P1

What do you recommend here?

[andrea.amilo · Accepted solution]

Hello @Anonymous,

your postprocessor is properly configured to use G68.2 function with 3+2 toolpaths.

Based on my Mazak programming knowledge, it could be possibile you need to replace G53.1 P1 with G53.1 P2 in case of B negative orientation. So G53.1 P1 if B positive, G53.1 P2 if B negative.

This is what I've found in a Mazak programming manual:

B. Tool-axis direction control
G53.1 Pp
G53.1: Tool-axis direction control
P: Selection of a solution for the axis of rotation.
0: Processed as “P = 1” or “P = 2”, depending on the construction of the machine.
Works the same as “P = 1” on this machine system.
1: Solution with a positive angle of rotation on the B-axis.
2: Solution with a negative angle of rotation on the B-axis.

You might try to edit manually your nc file to check if this is your machine configuration, too.

If so, we can update your postprocessor.

Please test it carefully and let me know.

[Anonymous]

@andrea.amilo   Yes....the P2 after 53.1 solved the solution.  I am changing this manually.  

How do I edit the post to automatically post P2 moves? 

Thank you sir

[andrea.amilo]

Hello @Anonymous ,

I think you need to write B and C preposition values before G68.2 to be able to check the proper B value.

If so, you can activate the useABCPrepositioning option at line 262 :

then you can define your IF statement to check B value, from line 820 to line 824 :

Please test it carefully and let me know.