Hi. I am using mach3. I have set up the table limits in the software.yet when the g code is downloaded the work always shows itself outside the table display. This of course means I cant cut the work.what am I doing wrong.
Printable View
Hi. I am using mach3. I have set up the table limits in the software.yet when the g code is downloaded the work always shows itself outside the table display. This of course means I cant cut the work.what am I doing wrong.
Terry Can you supply more info. Do you have home switches? Are you touching off and zeroing to the part on the table?Quote:
Originally Posted by terry1956
Hi.the machine does not have home switches.i zero the machine both touching x,y sides of work material and zeroing the drop in turn and the lowering the z axis until the mill end is a paper thickness from the material surface and then zero that axis.
How are you generating your gcode ie in the cad is the part at the X0 & Y0 postion.
put a sample of the gcode up. say the first 10 lines
Hi. Find second problem. Reading up on homing the machine on the mach3 forum. The write up states.move the spindle to the center of the bed. Press ref all and zero the dro. Then zero machine goords. Both sections should now read zero on all axis. Then go to off sets and check its reading G54 and the axis are also reading zero. But I cant get the machine goords to zero, and the off set will not allow me to reset the axis readings or change anything bar the press the machine goords button and zero that dro, but then it returns to the off set reading. What am I doing wrong. The g code was made using vcarve.but I think its the offset problem that needs sorting.
As I remember, you can only reset the machine coords DRO to zero if you have disabled all limit/home switches in Mach3. You then position the spindle to machine zero manually with the jog controls, then (I think) you hit "Ref All". I'm not absolutely sure about that last bit as I've only used it for testing when I was building my machine but I am pretty sure that you have to have all lim/home switches marked as disabled or Mach3 won't let you zero machine coords.
Hi, just an update. I think the fault lays within the older version of mach I am using. I have downloaded a newer version and the material offsets are zero.so I can now zero all dros. I am going to fit limit switches to the machine before trying to home the machine again.fingers crossed
Terry do you know the difference between home and limit switches. As there are various ways of using them. ie you can have switches just for the limits on the machine with separate home switches. or you can use a limit and home switch combined.Quote:
I am going to fit limit switches to the machine before trying to home the machine again.fingers crossed
manual http://www.machsupport.com/wp-conten...3Mill_1.84.pdf section 4.6
Whether or not you use them as limit switches as well, home switches are a great time-saver! Also means that you can sensibly use soft limits as Mach3 now knows where the machine table is.
Good luck!
Hi Terry,Quote:
Originally Posted by terry1956
Probably was corrupt install of mach3 but however I think your not fully understanding the process and what an Material offset means and how it's determined.
Material Offset is the distance from MACHINE COORD ZERO to WORK COORD ZERO.
When HOME switches are fitted they provide the Reference ZERO for MACHINE COORDS. Hence why when you push RefAllHome the MACHINE Dro's change to Zero. If you had switches fitted the machine would move towards them and stop when triggered, then Zero the DRO's.
As you have it now you can set MACHINE ZERO at any point by pressing "RefAllHome". This wouldn't be the case if "HOME" input was enabled because MACHINE ZERO is FIXED and never changes in relation to machine unless switch is moved.
Next you set WORK COORD ZERO by pushing ZERO X, Y, Z next to DRO's. This then creates WORK OFFSET distance and stores it in WORK OFFSET list.
Now here's where it can get slightly confusing and the G54 comes into play.?
You can have many WORK OFFSETS each with different WORK ZERO position, some times you'll see these called Fixture Offset's or Material Offsets it's all same thing.
This done using G54,G55,56, etc Now the default WORK OFFSET is G54. But could easily create another by typing G55 in MDI then moving to different position and push ZERO X, Y, Z. Now when you look in the WORK OFFSET list you'll see G55 has it's own set of Coords which show the distance from HOME.
Which in your case is the point where machine was parked when you clicked "RefAllHome". If you move the machine and Click RefAllHome again the WORKOFFSET doesn't change it will still be the same distance away from your new MACHINE ZERO.
To see this work try this. Park machine in place with plenty movement left in each axis and push "RefAllHome" this will ZERO the MACHINE COORDS. Now jog away some distance, say 20mm then ZERO WORK COORDS by pushing ZERO X, Y, Z.
Now without moving machine click RefAllHome again. You'll see the WORK DRO's change from Zero to the Distance you moved. Now there's button which says "GoTo Zero" just below DRO's when press this the machine will move to WORK ZERO which is the distance you jogged away from MACHINE ZERO or point you pushed RefAllHome and now the DRO's will be ZERO again.
This is the WORK OFFSET being used and will always be the distance from MACHINE Zero.
The Danger in this without HOME or Limit switches fitted is that if you push RefAllHome near the end of your machine travels and in the WORK OFFSET table there is WORKOFFSET saved then could crash if your G-code as G0X0,Y0,Z0 because will send to the COORDS saved in the OFFSET Table which to MACH is set distance from MACHINE ZERO which just happens to be off the table.
Now here's where it gets double confusing for some when we bring SOFT LIMITS into play.?
SOFTLIMITS are also referenced from MACHINE ZERO so if you set mach softlimits to the size of your table this applied in relation to MACHINE ZERO point. So again because you moved MACHINE ZERO by Pressing RefAllHome further up the table your Softlimit table size is taken from this point so at some point will run off the machine and Mach won't now anything about it until the Crunch.!!
SOFTLIMITS are great when HOME swtiches are fitted but can be dangerous if not used correctly and MACHINE HOMED before using. Double dangerous when NO HOME or Limit sw are fitted because MACHINE ZERO can MOVE and no way of stopping machine when runs off the table.
SO GET HOME SW FITTED ASAP.!!!!!
Hope this helps.
Switches on order.Will update when I have fitted them in.please bear with me
I've not read all the replies, but i had the same issue and it was because I had set the zero position in Fusion 360 in the wrong corner of the stock vs the one I homed to in real life.