PDA

View Full Version : Setting a start point.



jrob3rts
16-06-2012, 09:47 PM
No doubt this is a really simple question, but how do people usually set a start point?

I apologise is the term "Start Point" is incorrect, and if so, please correct me.

On my machine, my start point is set manually at "X" and "Y" being zero (I.e. in the corner of the workpiece and "Z" being offset so it's at the top of the workpiece. It's a tedious job and leads to an inaccurate starting position at times.

I suspect that a start point which is set regardless of the workpiece would be better and I change the starting position and offset in Cut2d which I use to generate the GCode.

Thanks for your time.

James

Jay
16-06-2012, 11:00 PM
Im struggling to understand your problem mate but i think what your meaning is that your cad cam program isnt starting where you set your machine datum is this correct?

jrob3rts
16-06-2012, 11:13 PM
Im struggling to understand your problem mate but i think what your meaning is that your cad cam program isnt starting where you set your machine datum is this correct?

Hiya,
Apologies for my poor explanation. I suppose it's not so much of a problem, more of whether I can improve my process.
The software starts at the place I define, and I place the material at that point beforehand, so just wonder if as an example it is best to mark an offset (say at 20,20) and place my workpiece there. I suppose the question also stems from changing the cutter where I quickly realised that the height is difficult to set without setting the "Z" to 0 and allowing the cutter to drop to the table and then tightening the nut on the router to keep the height as expected.
Hope that makes a little more sense.
James

Ricardoco
16-06-2012, 11:16 PM
No doubt this is a really simple question, but how do people usually set a start point?

I apologise is the term "Start Point" is incorrect, and if so, please correct me.

On my machine, my start point is set manually at "X" and "Y" being zero (I.e. in the corner of the workpiece and "Z" being offset so it's at the top of the workpiece. It's a tedious job and leads to an inaccurate starting position at times.

I suspect that a start point which is set regardless of the workpiece would be better and I change the starting position and offset in Cut2d which I use to generate the GCode.

Thanks for your time.

James

Ok let me get this right, what you are asking is how you can put a piece of stock onto your work surface and have the corner assuming its a right angle be at x=0.0 & y=0.0 every time yes?

Jay
16-06-2012, 11:18 PM
if you want to move to a position away from the job for a tool change then just program it as the following,assuming your using work offsets and work in the x- and y- direction.

G00G54X20.Y20.
M0.
set new tool here then restart your program.

All the above is doing is moving the tool away from the job for a tool change and stopping until you hit cycle start again.

The above will work if your using G54 to G59 offsets but would be differant if using G92.

Ricardoco
16-06-2012, 11:30 PM
ok here is what i did, right or wrong i put a piece of stock on the bed to see where i would put the corner of most of the stock i use, when i was happy i put in a 6mm drill and drilled several holes 10mm deep along the x axis 25mm spacing 6 initialy, then i did the same on the y, then i put some 6mm pins in the holes (old broken twist drills cut down to size 20mm) they were a nice tight fit, i then put my stock against them clamped it down then set my coordinates to x=0.00 and y=0.00 at the corner of my stock just once, to acheive this i put one of the 6mm pins in the collet chuck and carefully jogged to the edge of the stock x then set the x to minus 3 then did the same on the y. i then moved the x and y to the home limit switches and took note of the coordinates for the future.

Im sure there is an easier way but then it has never let me down since so i dont even think about it any more..

as for the Z and tool changes that would depend on what type of tool holding you have adopted.

Rick

Jay
16-06-2012, 11:35 PM
Please tell me you did this to a not so expensive machine and not a VMC because id cry if even so much as a spot drill hit my table by so much as 1 micron...lol.
What your saying is a good way of doing it if you dont want to be setting up everytime you take a vice on and off the machine but constantly working in the same area of the machine will wear the guides down over time while the rest of the guides are nice and new.

Ricardoco
16-06-2012, 11:41 PM
Please tell me you did this to a not so expensive machine and not a VMC because id cry if even so much as a spot drill hit my table by so much as 1 micron...lol.
What your saying is a good way of doing it if you dont want to be setting up everytime you take a vice on and off the machine but constantly working in the same area of the machine will wear the guides down over time while the rest of the guides are nice and new. I take it you didnt read anything into the part that said " 25mm spacing 6 initialy" i should have elaborated i know but that was going to be in another post and i have a 20mm sacrificial bed on my machine which i was also going to put in the same post, i didnt want to put a huge paragraph on the post confusing anyone but you are quite right and i cut from all over the place on my machine because i know where all the spaced out holes are lol

jrob3rts
16-06-2012, 11:41 PM
Rocardoco - Thanks for that. It makes sense and I was considering a similar thing but making use of the T Slots for one axis and maybe bolt a piece of acrylic cut like a set square for the other.

Jay - Good point about the wear in a specific area, I had not considered that. Suspect it will be fine for now as it's for hobby use but as and when I have more time to spend on the machine I will take this into consideration.

James

JAZZCNC
16-06-2012, 11:43 PM
In cnc there are 2 coordinate systems, Machine coordinates (MC) and work coordinates (WC).
MC relate to the machines fully movement extents and often defined by having home switch's which set the MC X0,Y0,Z0.
WC is the start point you choose when zeroing on the workpiece and the G-code or part defining the extents.

WC are also related to MC in that they are a known distance from MC X0,Y0,Z0. With home switch's on the machine it makes very easy to get back to accurate WC start point or any other known point on the workpiece by specifiying the offset from MC.

So if you only want to work from one position IE set distance from MC then you need a known start point. This would then become your X0,Y0,Z0 in WC.
This known start position is set by using work offsets which are represented in G-code by G54,G56,G57,G58,G59. The usual default work offset is G54 and most just use this which is basicly set when you manuely zero the WC DRO's.
If you want to define other work offsets then this is done in the control softwares work offsets table section saved under G54,G55 etc, you then basicly program the relavent offset IE:G55 and the machine knows it's distance from MC and goes there using this has it's WC X0,Y0,Z0.

So the process goes like this jog the machine to a point on your bed, in your control software you'll have a workoff set table. This table will have list of coordinates for G54-G59 choose one and save, this save the MC for the position the machines at now.
Now when you program the part at the begining or near the begining of the G-code there will be an entry for setting the machine up safe looking some thing like "
N01 G21 G40 G49 G54 G80 G90 G91.1" This puts the machine in a known safe state. Further down there will possibly be another line with G54 so selecting workoff set G54 and it's WC in the Workoff set table. . . So by now I think you'll have guessed what needs to be done to choose another WC location.? Yep change G54 to G55 etc.!!
Better still is to do this in Cam software, most decent software should let you choose work offsets.

Hope this helps.

Ricardoco
16-06-2012, 11:44 PM
Rocardoco - Thanks for that. It makes sense and I was considering a similar thing but making use of the T Slots for one axis and maybe bolt a piece of acrylic cut like a set square for the other.



your very welcome and i also did it the way you have suggested in the begining but i kept moving it so decided on the pins..

Ricardoco
16-06-2012, 11:47 PM
Now ill give you it in the way clever people put it lol



In cnc there are 2 coordinate systems, Machine coordinates (MC) and work coordinates (WC).
MC relate to the machines fully movement extents and often defined by having home switch's which set the MC X0,Y0,Z0.
WC is the start point you choose when zeroing on the workpiece and the G-code or part defining the extents.

WC are also related to MC in that they are a known distance from MC X0,Y0,Z0. With home switch's on the machine it makes very easy to get back to accurate WC start point or any other known point on the workpiece by specifiying the offset from MC.

So if you only want to work from one position IE set distance from MC then you need a known start point. This would then become your X0,Y0,Z0 in WC.
This known start position is set by using work offsets which are represented in G-code by G54,G56,G57,G58,G59. The usual default work offset is G54 and most just use this which is basicly set when you manuely zero the WC DRO's.
If you want to define other work offsets then this is done in the control softwares work offsets table section saved under G54,G55 etc, you then basicly program the relavent offset IE:G55 and the machine knows it's distance from MC and goes there using this has it's WC X0,Y0,Z0.

So the process goes like this jog the machine to a point on your bed, in your control software you'll have a workoff set table. This table will have list of coordinates for G54-G59 choose one and save, this save the MC for the position the machines at now.
Now when you program the part at the begining or near the begining of the G-code there will be an entry for setting the machine up safe looking some thing like "
N01 G21 G40 G49 G54 G80 G90 G91.1" This puts the machine in a known safe state. Further down there will possibly be another line with G54 so selecting workoff set G54 and it's WC in the Workoff set table. . . So by now I think you'll have guessed what needs to be done to choose another WC location.? Yep change G54 to G55 etc.!!
Better still is to do this in Cam software, most decent software should let you choose work offsets.

Hope this helps.

Cheers Jazz (copy & paste to notepad)

JAZZCNC
17-06-2012, 12:13 AM
Work offsets(WO) are very usefull if you have large bed. You can basicly devide the bed up into individual sections that can quickly and easily be located using WO.
If used in combination with fixture jigs and location dowels it makes for very easy multipart cutting using different materials of different thickness's which can be left unattended. Just combine the code in one long G-code file by copy and paste and when the control comes across the new WO G-code it will move to that point and start a fresh adjusting for the offsets.!

Great for doing things like 2 sided cutting on multiple parts using fixture jigs. Cut the first side in G54 and while this is cutting set another to be cut in G55. While G55 is cutting remove G54 jig from machine reset part for other side and replace back in G54 position for the other side. The code will be set in such a way that after the first twin same cut it flips back and forth between front and back sides. . . . . Obviously this is job dependent but you get the idea.!!

Jay
17-06-2012, 11:32 AM
no mate i missed the sacrificial bed part sorry but glad to hear your not drilling holes in the main bed..lol

Robin Hewitt
17-06-2012, 01:36 PM
I know exactly what you mean, I used to find this a right PITA because when you produce a G Code you lose the original drawing, in my case a DXF file.

To fix it I rewrote my cutting software to read in the DXF and every circle shows on screen with a little red rectangle in the middle.

Right button the rectangle and it sets machine co-ordinates to the circle centre, left button it and it moves the tool to the circle centre.

I can also click left or right anywhere on the drawing, which is handy to make sure the cut doesn't overhang the billet.

What I do is drill some holes for locating bolts then clear the mill bed of everything.

I have a bunch of 3/4" thick mounts which have a T slot fixing and an offset stud with a female thread. I made 4 of each in M3 M4 M5 M6 and M8.

I locate the mounts by left buttoning rectangles, lock them in place, replace the billet and bolt it down.

If I have clear space and remembered to add a spare circle to the drawing, I pop in a centre hole so I can relocate if I lose position.

Lots of typing but I would not be without it.

When I am not machining the outside of the billet and need to align metal to the bed, I use the 10mm square tool steel bar I inset a few mm deep at the back of the bed. I cut the pocket for it with the mill so I know it is dead square. It has a splash guard holder on the top.

If trying to align to a centre scratch I start light with a centre drill and go progressively deeper with each attempt to erase the old mark. Really need a sensitive drill handle and a pendant for that.