Productivity Plus

[gcode]

My bosses want to run a production part on our Mori Seiki NT 5X mill/turn
To run efficiently probing is required.

I know next to nothing about Productivity +
Is it a workable solution for a 5X mill/turn

[Hardmill]

Not sure but take a look at CappsNc.
We used it in El Segundo
I believe they still have the 3 seats in Camarillo

https://aat3d.com/">https://aat3d.com/





















PEACE

[Bob Sacamano]

Currently, Productivity plus does not work on Mill-Turn machines.

[JACKOFFALLTRADES]

Hi Tom,

Is there a reason you "have to" program the Probing Cycles inside Prod+?

Are you familiar with Probing Cycles to begin with?

I like Prod+ for the people who are already familiar with Probing, and want to simply integrate Probing Cycle Generation, and want the ability to visualize the Probe moves in Backplot.

If you are the kind of shop where "almost every part gets Probed", then Prod+ is a good investment.

I tend to write many of my Probing Programs "by hand-coding", because the process is generally so simple, and really "doesn't change much" once you've developed the cycle. Typically, I'll just code 1 or 2 "Manual Entries" at the top of my Ops Tree, and configure my Post to output the "Manual Entry Ops" in 'pheader$', while saving the Operation Comment output for 'psof$'. (This is due to the way that Mastercam 'codes' the Manual Entry paths as "comments", and adds these comments to the 'Comment Buffer'. Unfortunately, a "Manual Entry Operation", isn't coded as an "operation" in terms of the NCI File Formatting.)

Renishaw makes a Software Package called "Inspection Plus", which is a Standalone Software, which can be used to develop Probing Routines, and add them to 'processed NC Code', but Prod+ does the "same thing", within the Mastercam User Interface. (Less learning curve for Prod+).

If you just need to develop a cycle to "locate a part" > by setting a Work Offset, and you don't do this very often, then I'd simply code the Probing Cycles manually, using Protected Position moves to get "in/out" of the Probing Positions. Then you can use Single Point, Web/Pocket, or Bore/Boss Macro Calls, and pass in the options you need with the Parameters.

The "output" of the Probing Cycle is typically "setting the Work Offset Positions", but you can also read the 'Local Macro Variables' (#100-#149), after each Probing Cycle finishes, if you need to store or manipulate the Probing Results.

[gcode]

Is there a reason you "have to" program the Probing Cycles inside Prod+?

I am not familiar with probing and being chained to my desk ( and now working from home)
the opportunity to learn  probing at the machine is not there.

We have a Mori Seiki NT6000 mill/turn and a production order for a large square weldment
12" square X 10 ft long
It has lots of holes and simple mill features all coming off datums defined by various welded features.

We would like to fixture the part between centers, probe it,  setting a half dozen work offsets
and go to town.

I know that Productivity + does not support mill/turn  but Postability tells me they cam trick a mill/turn
into running Productivity+ with a horizontal mill machine definition running in a separate Machine Group.

That means probing code would have to be manually inserted into the machining file,
but I'm thinking 2 separate files. First run the probing file to set the work offsets, then run the machining file.

The machine was built in 2008 and has probing installed. I have Renishaw coming out next year
to see what is there and what we may need to add or update.
We bought the machine from a sister company who bought it for a failed lights out machining program.
The machine is 12 years old and has 200 hours on the clock.
 
Personally I have my doubts about the entire concept. IMO this is not the best use for a
very nice mill/turn.
However the project is being driven by upper management who will not take no for an answer.

To make matters worse, our MC dealer is not enthusiastic about the project, due to CV-19
restrictions and the technical issues involved.

[JACKOFFALLTRADES]

Since you have Renishaw coming out already, I would suggest contracting with them directly to write the custom Probing Cycles to set all the Work Offsets, and be done with it. They will make it work correctly, since this is a single weldment part.

If this was going to be a "well, we are going to do a series of 10 weldments, that are all similar", then that is where I'd investigate Prod+.

Setting each individual Work Offset, will only take the execution of "at most", 3 separate cycles. If you are picking up a Bore or Boss, then it would be 2 cycles for each Offset (1 for XY center, and 1 to find Z).

So, if you've got 6 Offsets to probe, that is (again, at most) 18 lines of G-Code that are needed to record the positions.

Granted, you'll want probably 2 extra G-code line (approach and retract in Protect Move) for each position, so a total of 30 lines of NC Code, to do the "actual Probing" on that part.

Of course that doesn't include things like Tool Change, TLO approach, or Safety Line, but you get the idea.

Most of my Probing Subroutines probably average 20-50 lines of NC Code, if all I'm doing is setting a Work Offset.

If you are Probing and then "outputting Probe Results" to a File, then you can get into the 100's or 1000's of lines of Probing Code, as there can be quite a few lines for just "1 feature" when you are outputting reports.

[Hardmill]

Honestly G look into CappsNc
You completely program offline and send to an execution station to run at machine





















PEACE