reposting of programs

[jim S]

We are running Mastercam with our Mazak Variaxis and I think our post is set up wrong. Each time we run a part, we have to repost the program. my operators are telling me that if the tooling isnt set up exactly the same as the previous time we ran the part then the program has to be reposted. Does anyone know if this is true and/or if the problem can be overcome?

[Colin Gilchrist]

Your operators are absolutely correct. As the tool lengths and part/fixture location change, the program must be updated to reflect these changes.

 

That said, there are software options on the machine's control that can be used to overcome these obstacles, but it depends entirely on if those options were purchased (or can be retrofitted) on the control. These compensation features are typically called "Dynamic Work Offset" or "Dynamic Fixture Offset". These are 3 + 2 options, which compensate for part/fixture not being located in the exact spot on the machine.

 

The other option is called "Tool Center Point Control" or "Rotary Tool Center Point", and allow the machine to perform "dynamic" tool length compensation. This is typically used to compensate for a "live" 5 Axis cut.

 

If these options are available on the machine, you will need to have your post modified to output the correct codes to take advantage of these options.

[jim S]

Colin,

Thank you! We are using dynamic offset for our workpiece coordinates. Is there something that has to be used in conjunction with this? We are doing very little "live 5" machining, most of our work is positional.

[Guest MTB Technical Services]

Your operators are absolutely correct. As the tool lengths and part/fixture location change, the program must be updated to reflect these changes.

 

That said, there are software options on the machine's control that can be used to overcome these obstacles, but it depends entirely on if those options were purchased (or can be retrofitted) on the control. These compensation features are typically called "Dynamic Work Offset" or "Dynamic Fixture Offset". These are 3 + 2 options, which compensate for part/fixture not being located in the exact spot on the machine.

 

The other option is called "Tool Center Point Control" or "Rotary Tool Center Point", and allow the machine to perform "dynamic" tool length compensation. This is typically used to compensate for a "live" 5 Axis cut.

 

If these options are available on the machine, you will need to have your post modified to output the correct codes to take advantage of these options.

 

 

Colin,

 

If this is a head-head or head-table machine then the answer is maybe,

 

The Vari-Axis is a table-table or dual rotary table machine.

There is no reason to re-post for a table-table configuration unless the part WCS has changed.

The tool length in Mastercam is essentially irrelevant for this type of 5-Axis as the XYZ point is the tip of the tool,

and the part is programmed referencing the center of rotation of the dual-rotary tables as the WCS.

 

All that is needed is to properly set the tool offsets.

Granted, the correct cut lengths, projection and holder style should generally match,

there is still no need to re-post unless you have made substantial changes to a tool assembly.

 

A head-head machine can also run without re-posting if it was originally running with TCP.

If not, then the XYZ positions in the NC code are the center of rotation of the head and any change to the established tool lengths

would require re-posting.

I only see this in old-school aerospace applications these days.

Most are running TCP these days on head-head machines.

 

Using TCP for table-table configurations is really only used to constrain the motion within the machine envelope

as TCP maintains the relationship of the tool to the workpiece. It doesn't have any other practical value for table-table machines.

Even with that, you must be very careful as it is very easy to reach max velocity on the slowest rotary almost instantly.