Help !!!!

zac · 2007-05-29 20:19:52

Hello everybody:

I have a favor to ask. Can somebody kindly tell me how to modify the M6 Macro for simens 840D control. The machine does some wierd motion at M6 (2 Independantly prgrammable heads). I would like to relplicate the same motion on Vericut Machine Sim. as there are other fixtures on the table and possible collision that I would miss. THE BAD part is that I have no experience in modifying the control file.

Thank you in advance

Regards

zac

stpendl · 2007-05-29 21:32:56

Here is a sample of a M6 macro with motion.

	WORD_VALUE "M" "6" {
			MACRO "RotationPlaneCancel"
			MACRO "ToolLengthCompOff" {
				AFTER_MOTION Yes 
			}
			MACRO "DynamicWorkOffsets" {
				OVERRIDE_VALUE 1 
			}
			MACRO "DynamicWorkOffsets" {
				AFTER_MOTION Yes OVERRIDE_VALUE 0 
			}
			MACRO "ZAxisMachineMotion" {
				OVERRIDE_VALUE 1300 
			}
			MACRO "ProcessMotion"
			MACRO "XAxisMachineMotion" {
				OVERRIDE_VALUE -604 
			}
			MACRO "yAxisMachineMotion" {
				OVERRIDE_VALUE 633 
			}
			MACRO "ProcessMotion"
			MACRO "ZAxisMachineMotion" {
				OVERRIDE_VALUE 1176.5 
			}
			MACRO "ProcessMotion"
			MACRO "SpindleMotionOff"
			MACRO "ToolCode"
			MACRO "ToolChange"
			MACRO "ZAxisMachineMotion" {
				OVERRIDE_VALUE 1300 
			}
			MACRO "ProcessMotion"
			MACRO "CutterCompToolNum"
			MACRO "ToolLengthCompToolNum"
			MACRO "ToolLengthCompPos"
	}

zac · 2007-05-29 22:03:02

Thanks for the reply Stefan..

Is it a simens 840D M6 macro ? does it make any difference if it is not .... I don't know ...well if it is what does the override values -604/633... stands for ??? At M6 at least I want the machine to go up to Z limit then to Y- limit ~ change the tool ~ come back to the same place with the new tool on the spindle ~ continue with the program. Can I attain this by changing any of the values that you have shown here......

DaveF · 2007-05-30 00:12:00

Zac

2 Independantly prgrammable heads

take a look at headchanger.vcproject

it calls c:\C:\cgtech bla bla \samples\headchanger.sub

if you load the sub in the project, rather than where it is imbedded in the control, you can single block thru the sub, and watch the logic step thru with edit tool path.

you can call if you get stuck

Dave

DaveF · 2007-05-30 00:20:35

Zac

also, you can also add a tool change position
g-code settting > tables

Yes, it is a Kluge, but it may do close to what you want.
dave

DaveF · 2007-05-30 00:49:50

Stefan

Thats a nice macro 8)

I have something similar, and I need to update it to soon, to store the X AND Y position as a variable before the M6 is called, and than return to those stored values after the tool change. Have you gone down that road?

Dave

stpendl · 2007-05-30 09:04:09

zac wrote:

does it make any difference if it is not .... I don't know ...well if it is what does the override values -604/633... stands for ???

There is nothing special about this macro, I modified the standard M6 macro to include the tool change moves along the machine coordinate system, since using the tool change position did not give the correct movement.

The override values are the positions the machine has to move to with the specified axis.
Insert "ProcessMotion" to let the machine move to the before defined positions.

stpendl · 2007-05-30 09:07:45

DaveF wrote:

I have something similar, and I need to update it to soon, to store the X AND Y position as a variable before the M6 is called, and than return to those stored values after the tool change. Have you gone down that road?

No, I have not had such a need by now.

We have only evaluated VC machine simulation and use UG IS&V now, since it is sufficient for our needs.

VERICUT Users' Forum

#1 2007-05-29 20:19:52

Help !!!!

#2 2007-05-29 21:32:56

Re: Help !!!!

#3 2007-05-29 22:03:02

Re: Help !!!!

#4 2007-05-30 00:12:00

Re: Help !!!!

#5 2007-05-30 00:20:35

Re: Help !!!!

#6 2007-05-30 00:49:50

Re: Help !!!!

#7 2007-05-30 09:04:09

Re: Help !!!!

#8 2007-05-30 09:07:45

Re: Help !!!!

Board footer