3+2 programming and tool changes

[KKlausman]

Hey everyone,

New here to the forum. I have a HAAS UMC 750. I am programming and machining a part that uses the same plane for multiple toolpaths and multiple tools. I am trying to minimize the amount of times my machine "homes" itself before it does a tool change when it is just going to grab another tool (safely) and go right back to the same position. Any help would be appreciated.

Thanks,

Kevin

[Colin Gilchrist]

32 minutes ago, KKlausman said:

Hey everyone,

New here to the forum. I have a HAAS UMC 750. I am programming and machining a part that uses the same plane for multiple toolpaths and multiple tools. I am trying to minimize the amount of times my machine "homes" itself before it does a tool change when it is just going to grab another tool (safely) and go right back to the same position. Any help would be appreciated.

Thanks,

Kevin

It sounds like you'll need to work with your Post Processor Developer to make some edits to the G-code, unless I'm misunderstanding what you are asking.

But, that also depends on your setup.

A new feature available on the UMC machines is the "mid-point for Tool Change". So when you execute a Tool Change, if there is a tall fixture/part in the machine, you can force the Machine to go to any XYZBC Position, before the actual "M06" is called.

For each Machine Axis, you have the ability to specify a "specific machine location", or set the option to "inactive", which means that you can use the "mid-point for tool change", on a "per-Axis" basis.

Are you looking to change how the Tool Change "safe mid position" executes (disable the mid-point so the Tool Change executes faster), or are you looking to minimize or change the NC Code that you are outputting from Mastercam?

 

[civiceg]

Quote

A new feature available on the UMC machines is the "mid-point for Tool Change". So when you execute a Tool Change, if there is a tall fixture/part in the machine, you can force the Machine to go to any XYZBC Position, before the actual "M06" is called.

This has been around for many years on a Haas(15+). It was just parameters using encoder counts to preposition to the location before a tool change. Much easier on a NGC though. Exact same functionality. You could also alias an M6 or do a combination of both. 

Most UMC post have a misc integer to not go to the "home position" during mid op rotations and also at the start/end of the operation.

Postability, IHS, and I even believe the Mastercam Direct post also has a misc integer for it. 

Just have to make sure your retract plane is high enough when turned off. 

[DUM1]

I have the same thing,  but it seems that if I use a duplicate wcs top for my main rotations instead of the master top wcs the homing for every tool change lessons , but I haven't nailed it down yet  . because it seems to work sometimes and not others.

[KKlausman]

Colin/Civiceg,

I do not know anything about the "mid-point for tool change" so I would have to read up on that and learn how to utilize the feature. (If it pertains to what I am trying to accomplish) With that said, I am not necessarily trying to make the actual tool change happen faster. (the speed of the tool change is fine) What I am trying to do is keep the trunnion and platter from going to their home positions every time the machine does a tool change.

Let me try to paint my picture.. (bare with me) Imagine I have 1 surface with 3 sets of tapped holes and each is a different thread. That would mean 1 spot drill, 3 different drill bits, and 3 different taps. The trunnion and platter rotate to a certain angle I call out for that surface to start the spot drilling for all holes. I want the trunnion and platter to stay exactly where it is while the machine does the next 6 ops and tool changes in order to finish the holes. Right now the trunnion and platter are zeroing and re-positioning 7 times just to go to the same exact spot again and again.

B0. C0. to B90. C180. then back to B0. C0. then back to B90 C180. (over and over) Seems like a big waste of time to me.

I have the Postability post and have looked into the integers but nothing seems to work. I actually have my CAM retailer looking into it as well to see if they can add the integer you are referencing.

 

[Colin Gilchrist]

Good, you are going down the right path for figuring this out.

• Are these "rotations": B0. C0. to B90. C180. then back to B0. C0. then back to B90 C180.  called out in your NC Code (I.E.; the program is telling the machine to make these moves)?
• The "mid-point point for tool change" function can make the machine add "extra" rotations, when no rotary commands are given in the NC Code.

Just to eliminate the possibility that "mid-point for tool change" is causing the issue, I recommend you set the Rotaries to "Inactive", so that we can eliminate one variable as being the cause. But if you are getting the B0. C0. then B90. C180., and so on, output in the actual NC Program, then you'd need to have the Post edited.

To disable just the "rotary" movements for the Tool Change, use the following procedure.

WARNING: When changing settings like this, there is a possibility of machine collision if you aren't paying attention. I'd recommend running through the program in Single Block, with Rapid Override set at 5%, until you are certain that the changes to "Tool Change Mid Position" still give you clearance during the actual tool change. This can be especially problematic if you test with a "shorter tool", and then have a long tool later in the program!

To disable "Tool Change Mid Position":

• Press the "Settings" button twice. (Be sure you have the "tabs" highlighted at the top of your operator screen.)
• Press Right Arrow button, until you have the "User Positions" tab highlighted.
• Press Down Arrow to enter the "user positions" menu, and continue until "Tool Change Mid Position" is highlighted.
• Press Right Arrow to enter the "Tool Change Mid Position" settings.
• There will be 6 available axes that can be assigned a "Machine Position", or can be assigned to "Inactive". The "inactive" part is what you want for the rotaries.
• Press Down Arrow, until the 'Tool Change Mid Position B' is highlighted.
• Press the "ORIGIN" button on the Control. The Control will prompt you with a Warning: press "1" to change this individual setting, or press "2" to change all settings in this group. 
• Press the "1" button (on the 10-key keypad), to set the 'Tool Change Mid Position B' to 'inactive'.
• Repeat the same steps with 'Tool Change Mid Position C'. (Set to 'inactive'.)