Is Mazatrol 3+2 without CAM possible?

[AlexScott]

I have many Mazak machines (36 horizontals w/ 2 pallet changers, 1 palletech system hooked up to two horizontals, and 4 variaxis). Two of the Variaxis' are new with full 5 axis capability and Smooth Control. I understand CAM is king for 5 axis work and nearly impossible to live without. I use MasterCAM with custom posts for the full 5 axis work and understand how it works, but still want my programs in Mazatrol so everyone in the shop can understand them and make little adjustments to programs when needed with ease.

 

I am wondering if there is a way to use Mazatrol for 3 + 2 work without setting zeros for each face (cheating they say). So if I have a part with 5 sides to be machined (3+2), I set multiple zeros, one for each face, and that works fine. Is there any way in Mazatrol to set only 1 zero (just like I would when using mastercam and G68.2) and have the machine know where the workpiece is after rotating?

 

Pretty sure it has something to do with WPC SHIFT.

 

Thanks in advance.

[JParis]

We have

21 Mazak HMC's across 6 Palletechs lines

10 Mazak VMC's

10 Mazak 100 & 200 MSY's

3  Mazak i100 Integrex's

1 Mazak VC300A/5X

Everything except the MSY's are driven with Mastercam...

Don't know what kind of work you do but we could never drive everything with Mazatrol.

 

 

 

[cncappsjames]

If I had CAD/CAM at my disposal, I would NEVER use conversational on a mill except as an ABSOLUTE last resort.

That just defies all logic IMHO.

[huskermcdoogle]

9 minutes ago, cncappsjames said:

That just defies all logic IMHO.

Except the logic he presented forth....  He has good intentions, but....  

I'd want the parts to be super simple, mostly just hole poking type work, I mean really simple 2.5d work.  Otherwise machines will be sitting all the time while operators fat finger their programs at each setup.

I do believe WPCSHIFT is what you are after.  Your best bet would be to get a local apps engineer in from your dealer and have them work out a programming sequence with you.  With that many machines on your floor, surely you can get them to come in and help....  Likely for free if it can be done remotely, which in reality shouldn't be a problem.

 

But I still say WHY?  Are the operators programming the simple stuff at the machine?  If so, there are potentially much better ways to operate a shop, then again, we don't know what type of business your shop does, maybe it works pretty well.  Based on how many machines you guys have, it seems to do pretty well.

 

 

[Guest]

I've seen some really well implemented shops using Mazaks doing only conversation programs, but they weren't doing 3+2 ops..

[Matthew Hajicek - Singularity]

As said above, I could maybe see it for super simple 2.5D parts, but you'd better hope each machine operator is a whiz at Mazatrol.  Just remember that each minute the operator is programming and debugging at the machine is a minute of lost production.  Program it offline, run it through verification, and it's ready to go when the machine is done with the previous part.

[cncappsjames]

23 hours ago, huskermcdoogle said:

Except the logic he presented forth....  He has good intentions, but....  

...

But I still say WHY? ...

This... ^^^^^^^^^

I've got a customer with probably 30 Mazak VMC's. They do a lot of part family type work. They still do all their programming offline. Revision control, process control, tool library control, etc... in this day and age, conversational programming for all but the simplest of parts just doesn;t make a whole lot of economic sense. At least from my seats.

[Colin Gilchrist]

What would it take to automate most of those machines in your shop, to use a Renishaw Probe to help eliminate the "fine tuning" that is being done "at the machine".

With a good 5-Axis Post, and a (5-Axis) Probing System you should be able to do the following:

• Run a routine to set Center of Rotation parameters. < This should be done "often", depending on your tolerance needs. Some shops will be 'monthly', others are 'weekly', some are 'every morning',  and some processes require "calibration to different tolerances with the Probe", before a critical feature is cut. (in other words "it is different for everyone, but should be a regular and commonly done process in your shop.)
• Once the C.O.R. is calculated (correctly), all the "good 5X features" work by allowing you to program "From a Work Offset Location". < This means you get to Probe the Stock or in-process part, to set a Work Offset value, with the machine rotaries at zero. That is your Active Part Offset (Work Offset).
• 5-Axis Cuts will all use that Work Offset, with Tool Center Point Control. This gives you "Dynamic Tool Length Compensation".
• 3+2 Cuts should all use "G68.2 - TWP" for location. Here is where a "good Post" is separated from an "ok Post". You should be able to set a "Feature Zero Location", so that the G68.2 Line has an XYZ Offset, to move the G68.2 Origin, to the "face that will be perpendicular to the Spindle.". 
• When a 5-Axis is configured correctly, you should be able to use G41.1&G42.1 (or any number of .x suffixes, for example G41.5 & G42.5), to get "5-Axis Vector Compensation". You're not getting any "full 5-Axis Cutter Comp", with Mazatrol!
• IF you offset the Origin with G68.2, you don't have to worry at all, about re-calculating a new Work Offset for each face.
• This would give you the advantage, of making your Drill Cycles easy to edit at the machine. (For example, to change a G84 Z-0.625, to G84 Z-.75, is an easy change for the Operator to make.
• They can still change Speeds & Feeds, although "probably not as easy as changing in Mazatrol", especially when making a "global edit", but the Editor can handle EIA code. Ideally, that feedback from the Operators would go back to the Programmer, so they could fix the Mastercam Operations, and output a new NC Program that is error-free. This is the best option for any shop concerned about Revision Control.

I understand that your shop, and many of your Operators have been successful up to this point, creating and using Mazatrol Programs, but I would highly recommend doing some internal training for your company, and get everyone familar with EIA codes.

• Running EIA format (Posted NC Code), allows you (in the programming office), to control different High Speed Modes for those machines.
• All of the EIA Code that Mazaks run, is very similar to Fanuc NC Code formatting, and is basically what the industry uses "standard".
• The part or fixture can be moved anywhere on the table, and the Probe can then set the Work Offset location. All of your 3+2 features are now "location controlled by TWP".
• For "critical features", you can always elect to use a "secondary work offset", and just programmatically copy the G54 XYZ > G55 XYZ, before running the process. (Do this with Macro Variable code, in the NC Program, to automate the process.
• Call "G55" before "G68.2", and then use the G53.1 and XYZ move, to get the Probe in position. (The G68.2 "origin shift" now gives you a new XYZ Zero, that has been shifted over to the part face.) But now the Probe comes into play, because we can measure a critical feature like an existing face or bore, and "update the G55 Work Offset", based on the Probe results.
• We now "cut any of those features at G55, that need to be in the correct(ed) location.
• After we finish with those features, we recall G54, and then keep using G68.2 for all the other "less critical features".
• In necessary, you could "re-use" G55 many times, by simply "copying G54 XYZ > G55 XYZ", and then 'probing the new feature', after calling G68.2 and Positioning.

[nickbe10]

On 12/29/2020 at 2:16 PM, Matthew Hajicek - Conventus said:

Just remember that each minute the operator is programming and debugging at the machine is a minute of lost production

Spindle double whammy, you are bleeding at 2x rate, it just isn't good.