Enable HPCC G05 P10000 in MPMaster

[Bret Vanderhyden]

I have searched the forums on how to enable HPCC in the post, but I have only found this thread: http://www.emastercam.com/board/topic/71735-aicc-g05q1-how-to-enable/?hl=hpcc#entry834720

It is helpful, but only shows where to enable HPCC in the misc values tab from within the parameters of a given toolpath. However, I see that there is a check box on the misc values tab that says 'Automatically set to post values when posting'. Is it possible to configure the post so that HPCC will be automatically turned for all toolpaths that support it, instead of having to individually enable each toolpath?

 

Also, I did post out a toolpath with HPCC enabled in the misc values tab, but G05 P10000 was added after G43 -- Aren't all tool length offsets supposed to be canceled before HPCC is enabled, which would mean that g05 P10000 should go before G43?

 

thanks

 

Bret

[Guest]

I am running on a Robodrill the G05 P10000 is on the line right after the G43 and before the G49, G5 P0......have not experienced a single issue 

[crazy^millman]

I have searched the forums on how to enable HPCC in the post, but I have only found this thread: http://www.emastercam.com/board/topic/71735-aicc-g05q1-how-to-enable/?hl=hpcc#entry834720

It is helpful, but only shows where to enable HPCC in the misc values tab from within the parameters of a given toolpath. However, I see that there is a check box on the misc values tab that says 'Automatically set to post values when posting'. Is it possible to configure the post so that HPCC will be automatically turned for all toolpaths that support it, instead of having to individually enable each toolpath?

 

Also, I did post out a toolpath with HPCC enabled in the misc values tab, but G05 P10000 was added after G43 -- Aren't all tool length offsets supposed to be canceled before HPCC is enabled, which would mean that g05 P10000 should go before G43?

 

thanks

 

Bret

 

Yes, but that would be a pretty good post modification. You would need to create a turn on condition checking all of the toolpaths that could use and not use it. Then you would need to make sure you make a flag telling the post it was turned on and then make sure that flag turns it off. You can go into the post and make a simple modification that will make values in your misc reals always be there if you want to try that. Most posts are setup to error check operations where the HPCC should not be called and not output it.

 

Here is it is from one the posts we get from Postability:

[misc integers]
1. " "
2. "Abs/Inc, top level [0=Abs,1=Inc]"//0
3. "3D Comp (Surface Normal) [0=No,1=Yes]"//0
4. "Start Solution [0=-Tilt,1=+Tilt]"//0
5. " "
6. "Unit/Rev Feed [0=No,1=Yes]"//0
7. "Rotary [0=Post,1=Lock,2=Brake,3=Off]"//0
8. "Tilt [0=Post,1=Lock,2=Brake,3=Off]"//0
9. " "
10. "M0 Before Operation [0=No,1=Yes]"//0
[misc reals]
1. "CYCLE832 [0=Off,1=FINISH,2=ROUGH]"//1.//1.
2. "Accel/Decel Value [0=No Output]"//0.0254//0.0254
3. " "
4. " "
5. " "
6. " "
7. "Start Op Ret [0=Axis,1=Z,2=Z/XY,3=No]"//1.//1.
8. "Mid Op Ret [0=Axis,1=Z,2=Z/XY,3=No]"//1.//1.
9. "Rot Start [1=Value,2=Last,3=Rev,4=Prompt]"
10. "Rot Start [Enter Value or Rev]"

The //0//0 or //1//1 will force that into your misc reals areas for all operations. Then if the post is configured to not output it when you don't need it then all is good. Where you need a certain value you can do like the example //.0254//.0254 to force .0254  in the mr 2 box for all operations.

 

Bret, I am sorry to say this but, your second Question is completely wrong. You have asked about G05 P10000 which turns on HPCC. It does not turn it off. G43 enables tool lengths on every machine I have every run not turn them off. Like John said the G05 P0 turns off all HPCC and since the G49 which is turn off Tool Length Compensation is before it then everything is correct. What specific alarm or problem on the machine have you seen that makes you question what is going on?

 

HTH(Hope that Helps)