Haas PRE NGC Post Processor help with tapping

[raceman17]

I am having issues with tapping on my haas machine.  The issue is after a tap cycle the spindle does not orient back to the correct location.  So what happens is when the tool arm comes into change the tool the spindle dogs are not in the correct orientation and the tool jams in the tool swing arm/spindle.  This action only happens after a tapping cycle.  After all other tool changes the machine will orientate the spindle dogs to the correct location.  I tested this by adding a M19 code after a tap cycle and the machine orientated the dogs to the correct location and then the next tool changed worked as usual.  If the spindle does not orientate back to the correct location the tool will jam or the swing arm will not contact the tool in the correct location.  This results in the tool being thrown from the tool arm.

Can anybody provide some information on where/how to add a M19 spindle orientation code to the post processor so I do not have to manually add the M19 to the post.  I have near zero experience with modifying a post so any help would be greatly appreciated.

Thanks 

[Ariel]

M1
T92M6
S795M3
G54
M11
G0A-90.
M10
M8
G187
G0X-245.5Y57.8
G43Z80.H92
T140
G1F12700.
Z70.
G98G84X-245.5Y57.8Z37.5R52.5F771.15
X-94.5
X94.5
X245.5
G80
G1Z80.F12700.
M9
M5
G53G0Z0.

Here is a copy of one of my tapping cycles I am currently running on a Pre-NGC controller. Has worked for me from day one without any tool changing issues. Hope that helps

[engineguy]

@raceman17 

Are you using the latest version of the PP?

It is possible that you are missing the G80 after the Tapping cycle, is that in your code?

If there is no G80 then the Tapping mode won`t be cancelled, it is not normal to see an M19 command in G Code, it is normally done when other commands are called.

Is your PP like this ? Open in Visual Studio or any Text Editor and look for this area.

 Tap code same here as @Ariel  posted so unless there is some magic parameter not set in the control then, apologies, nothing more for you 🙂

[raceman17]

Yes, I'm using the latest pp. My post prosser gone also looks like what you mentioned. I am getting the g80 after the tap cycle. Maybe u have a parameter off in the control 

[engineguy]

@raceman17 

If all those are correct then it looks like there is a problem at your HAAS control, can`t help you with that I am afraid.

@Ariel  says the PP is fine his end!!

[mattdlr89]

Adding M19 in the post should be relatively straight forward. Perhaps if you attach the post here someone can help you edit it. 

I agree with what others say it doesn't sound right that you need to put an M19 in your post to do a tool change. I'd be inclined to figure out the root of the problem (I don't have experience with pre-NGC Haas) incase there is an error with your control/some settings that can fix it. Rather than patch up with a post edit. 

[programming2C78B]

Don't forget to check your setting 133, repeat rigid tap,

[raceman17]

setting 133 is enabled

[raceman17]

Here is a copy of my post.. I called haas this morning.  THey thought I had a software issue that something was not loaded right when I got the machine a few months ago.  Either that or a processor is going out.  Reguardless.. they want about 750$ to reload the software,  Everything else works as planned so it would be cheaper to figure out how to easily have the M19 command after a tap cycle.  Can anyone help me with the post?

[engineguy · Accepted solution]

@raceman17 

Well, to be brutally honest IMHO the $750 would be money well spent to have your control working as it should !!

Is this what you are looking for ??

I got it to post after the G80 and it outputs the M19, however that is set to post after the G80 and it posts on Drilling and Tapping cycles, up to you if you want to try it out in Fusion butI have no idea what it will do to your control, HAAS controls are "sensitive" at best to changes !!!

Usual caveat applies, use at your own risk and if doing it at the machine do it "in air" !!!

[raceman17]

yeap this it what I am talking about.  It really wont matter it it does a m19 after a drill cycle.  I defintely will try it out  My machine is at my house shop and not in a business so I'm really not making money off the machine.  Its just for home projects.  Haas was going to see if they could give me a deal on the software update if they can have a tech swing by the house and update the software.  I will report back and let you know if it works.

Thanks

[raceman17]

I just went a ran a program that hade several different milling operations switching between drilling and tapping and cutting.  Zero Issues!  Thank you!