G68 Rotation programming concerns

[csharp]

We are using a probe cycle to measure a machined flat on a round part and it stores the angle from the x axis in variable #139 and the error in #144. The part is held in a 3 jaw chuck mounted flat on table. Machine is a DNM5700. Since the measurement is from zero degrees the error and the angle are the same number.

I then use #144 to set the G68 rotation. If we run the program all the way through there is no concern. However if we want to jump ahead in the program to re-run a thread mill the #144 has been reset.

One solution we read was to write #501=#144 and the set G68 to #501. This way we maintain the value for rotation even after a "reset" or M30.

What are some possible issues with doing this? Is there a better solution?

Thanks

 

[sakis]

None. You have the solution.

 

[Vancbiker]

Depending on what control you have, there is a parameter that determines whether or not the #100 series common variables are cleared or retained at reset button push or M30.

 

[sinha]

What are some possible issues with doing this?

None, as long as you are aware that permanent common variables may have some initial values in the beginning of the program, and the same variables may have been used in several programs. It is a good practice to maintain a record of the purpose of all the used permanent common variables, so as to avoid unintentional updating of the values stored in these.

 

[dandrummerman21]

Some probes (renishaw, at least) use #501 for things. #501 is the radius of the ball iirc.

So i would be using one that is less likely to be used for something else, even if your machine/probe doesn't use it.

I use #668 for the purpose of G68, easy for me to remember. If you don't have extended macro variables (thru #999), I suggest you get the option.

 

[csharp]

Thank you all for the help.

Some probes (renishaw, at least) use #501 for things. #501 is the radius of the ball iirc.

So i would be using one that is less likely to be used for something else, even if your machine/probe doesn't use it.

I use #668 for the purpose of G68, easy for me to remember. If you don't have extended macro variables (thru #999), I suggest you get the option.

I am reading through our inspection plus manual for Fanuc(Doosan).

It does appear that the #501,#502 etc... are used or xradii, yradii ect....

I have not found where it states what range of variables that renishaw uses. I want to pick some outside of the ones they are using.

What was strange was there were no values in the #500, #501 when I went to use them.

I checked on the control and we have #100-#199 and #500-#999 available. As I scrolled through them I also noticed that #750-#759 had values in them. Makes me a little concerned that I may pick one that gets used by something else.

 

[sinha]

One way to ascertain if a permanent common variable has already been used, is to compare it with #0. If the equality is FALSE, choose some other variable. In the end of the program, reset the chosen variable to NULL (e.g., #500 = #0).
If you wish to retain the value stored in the chosen variable then more information about is use is needed.

 

[angelw]

I checked on the control and we have #100-#199 and #500-#999 available. As I scrolled through them I also noticed that #750-#759 had values in them. Makes me a little concerned that I may pick one that gets used by something else.

Let's just say that all of the Common Nonvolatile Variables were being used and none are available. A machine like yours is normally equipped with a multitude of Tool Offsets and in the event where a value needs to be retained when power to the control is cycled, but no Common Nonvolatile Variables are available, a Tool Offset can be used as a Variable in your program, just select the Offset Number that is least likely to be used and dedicate that Offset for use as a Variable. Probably the highest number Offset would be the most likely to use as its the least likely to be required as a Tool Offset and easiest to remember not to use as a Tool Offset. In your program, the System Variable for the selected Tool Offset for use is used in the program.

Regards,

Bill

 

[CNC Hacker]

Thank you all for the help.



I am reading through our inspection plus manual for Fanuc(Doosan).

It does appear that the #501,#502 etc... are used or xradii, yradii ect....

I have not found where it states what range of variables that renishaw uses. I want to pick some outside of the ones they are using.

What was strange was there were no values in the #500, #501 when I went to use them.

I checked on the control and we have #100-#199 and #500-#999 available. As I scrolled through them I also noticed that #750-#759 had values in them. Makes me a little concerned that I may pick one that gets used by something else.

Usually program 9724 will list what the base renishaw variable for calibration data is.

 

[sinha]

If more than one persons are using the same machine, then one may not know what others have done, with regards to permanent common variables. There should be a common protocol,

 

[csharp]

Thanks again for the help.

I was able to speak directly with a Renishaw rep. He explained that if I run through RenGUI that it is a compiled system and does not use the 500 variables.

They also indicated if I use the M165 calls instead of the G65 calls they compiled system is also called and not the #500 variables.