Using offsets
- Thread starter dsherburn
- Start date
tayloredtech
TayloredTech
Yes, from memory you would type G0 G55 X0Y0Z0 to send the machine to those co-ordinates.
I was about to post another question re offsets but I'll wait until this is confirmed
breezy
Moderator
Also you place G55 in your gcode and all following code is referenced of that location.
Typing G55 into the MDI will make all following manual commands reference that location but if you run a program that has placed G54 in as default this will override your manual setting.
If you are using Fusion 360 to generate your gcode you can tell it which G offset you want to use in the Setup dialog WCS tag. Offsets 0,1 are G54 and 2 onwards is G55 onwards.
Regards,
Arie.
Typing G55 into the MDI will make all following manual commands reference that location but if you run a program that has placed G54 in as default this will override your manual setting.
If you are using Fusion 360 to generate your gcode you can tell it which G offset you want to use in the Setup dialog WCS tag. Offsets 0,1 are G54 and 2 onwards is G55 onwards.
Regards,
Arie.
tayloredtech
TayloredTech
Awesome info thanks Arie,
Do you use Fusion and Aspire? I could use a man with your Gcode and camming talents. do you have Insta or another messaging service?
I do have a frustrastion with Masso I'm not sure if it's just my lack of knowledge or not.. possibly you could help. I will make a new post and tag you if that's ok.
Mitch
breezy
Moderator
I have been playing around with Fusion for a couple of years now, mainly with the CAD side and CAM only since we got the CNC router working at the shed. Have been looking at lots of Youtube about Fusion and picking up little tricks here and there.
The shed will get a copy of VCarve Pro in the future, so I'll have to get my head around that.
Currently I'm trying to understand SheetCam because we are mainly working with sheet material.
I don't use any messaging services other than email, you can get me at bms dot cncrouter at gmail dot com. That's the shed's email but I only attend on Mondays.
Dan,
As I explained in the other thread by TayloredTech. I have G54 set to a zero point on the router bed that is the corner of sheet stock. But when I want to use a different point on the sheet as the zero point I tell Fusion to use G55 and then when I load the program, I position the spindle on my G55 point and in MASSO F4 tab set G55 to the current position.
So for you to keep your gcode generic you will have to reset you G54 in MASSO F4 to the current location when you have clamped your part and moved the spindle to the parts zero point.
Regards,
Arie.
testyourdesign
testyourdesign
@dsherburn
Most CNC machines use home switches to establish an origin on the machine and soft limits to establish the work envelope for the machine. The work offsets (G54 through G59) give you a way to save the coordinates for a reference location inside your work envelope and call it up in your program using the G54 through G59 work offset reference. That way you can program your part using a known location on the part without worrying about where it is on the machine. This gives you more options when you want to use different size stock or various size machines.
The DRO buttons give you a way to save a temporary offset location called G92. The syntax for G92 temporary offsets are explained here. If you see the G92 number at the bottom of the screen then you are in temporary offset mode. To get out this mode you simply open the MDI panel and enter G92.1 to return to G54 mode. If you want to use the other work offsets you can activate them the same way using the MDI panel and typing in the G55 through G59 numbers.
I find DRO buttons useful when setting up my machine to align it with a specific feature on a part. In an example setup that already has hole in it I would:
After that you can then press the DRO button again or simply use the G54 table to save the new location. To save that new location I open the work offsets table and set the G54 offset value for that axis using the autoload feature. Once the G54 values are set I include a G54 command at the start of the G-Code program so that it goes to that location.
Its important to note that Masso defaults to G54 on startup so whatever value is set for G54 in the table will be the location that it starts cutting from when you start the program. If you don't enter G54 in your program Masso will still start that either the G54 location or the G92 location if its active.
I was confused by this at first also. With a little practice this will become second nature. Hope this helps.
Cheers, Stephen Brown
Most CNC machines use home switches to establish an origin on the machine and soft limits to establish the work envelope for the machine. The work offsets (G54 through G59) give you a way to save the coordinates for a reference location inside your work envelope and call it up in your program using the G54 through G59 work offset reference. That way you can program your part using a known location on the part without worrying about where it is on the machine. This gives you more options when you want to use different size stock or various size machines.
The DRO buttons give you a way to save a temporary offset location called G92. The syntax for G92 temporary offsets are explained here. If you see the G92 number at the bottom of the screen then you are in temporary offset mode. To get out this mode you simply open the MDI panel and enter G92.1 to return to G54 mode. If you want to use the other work offsets you can activate them the same way using the MDI panel and typing in the G55 through G59 numbers.
I find DRO buttons useful when setting up my machine to align it with a specific feature on a part. In an example setup that already has hole in it I would:
- Jog a probe into a hole with G54 active
- Slowly move along an axis until I contact the edge of the hole on that axis.
- Then press the DRO button to zero on that point to activate the G92 temporary work offset.
- Then move in the opposite direction until it contacts the other edge and note the distance measured on the DRO.
- Then I would use the G01 command to move half that value away from that edge and repeat in the other axis to accurately find the center of the hole.
After that you can then press the DRO button again or simply use the G54 table to save the new location. To save that new location I open the work offsets table and set the G54 offset value for that axis using the autoload feature. Once the G54 values are set I include a G54 command at the start of the G-Code program so that it goes to that location.
Its important to note that Masso defaults to G54 on startup so whatever value is set for G54 in the table will be the location that it starts cutting from when you start the program. If you don't enter G54 in your program Masso will still start that either the G54 location or the G92 location if its active.
I was confused by this at first also. With a little practice this will become second nature. Hope this helps.
Cheers, Stephen Brown
Thanks Stephen-good explanation. I do use home limit switches and the G54. I normally will use G92 offset after jogging to make sure my part fits in the job material I have loaded. The reason I was wondering if I could "pre-load" a G55-59 is that I have a grid of 20mm holes on my spoil board. I use the Kreg (and others) clamping and positioning dogs to locate and clamp material anywhere on my 4'x8' router bed. I could create offsets where the bottom left (for example) corner of the work piece would be located, based on where the Kreg dogs are in the various 20mm holes. I could then load one of my standard G codes from Vcarve, deploy a G55 from a MIDI command have the router machine the part where I have it placed. I currently do the same thing by jogging the machine to the piece, zeroing the x and y axis (creating G92) and starting. Works fine -just takes longer.
Regards-Dan
Regards-Dan
testyourdesign
testyourdesign
Hi Dan,
Definitely can us the G54 to G59 that way. All that you need to is move to the start spot you want and use auto load in work offset table to record it in memory. Probably need to mark the spoil board with the work offset number so you can find them.
To use it that way you simply open MDI and enter work offset number to activate it then enter G0 X0Y0 to get there.
Just remember to include that G54 to G55 number in the program or zero the DRO to use G92 before running the program.
Cheers, Stephen Brown
Definitely can us the G54 to G59 that way. All that you need to is move to the start spot you want and use auto load in work offset table to record it in memory. Probably need to mark the spoil board with the work offset number so you can find them.
To use it that way you simply open MDI and enter work offset number to activate it then enter G0 X0Y0 to get there.
Just remember to include that G54 to G55 number in the program or zero the DRO to use G92 before running the program.
Cheers, Stephen Brown
testyourdesign
testyourdesign
Yeah that's all it takes to move to that work offset but it would be allot easier to simply add a G55 near the start of your program instead. It takes care of moving to that location for you. All mine include a G54 or G55 at the start of the program.
Cheers, Stephen Brown
Cheers, Stephen Brown