Setting up the 0,0 point for a job . . . .
 

Copied from elsewhere . . . .

Jig shown for holding the location of "blanks"

I Still Battle To Get A Proper X-0/y-0 On My Table To Start Working From.
As Can Be Seen On The Table There Is A Square That Holds My Project In Place.
Did The First Cuts With No Hassle But As I Placed The Second Parts To Be Cut It Did Not Start Cutting In The Same Place.i Did The Cuts The Next Day So X0,y0 Should Be The Same.

On the 0,0 issue...Before you switch off for the night, make sure Mach3 show x=0 and y=0...z so that you can zero the next day. Leave your gantry where it stopped on the 0,0 position.
The next day switch everything on and Zero x and y on Mach3 or do as I usually do...drill a little hole with the router where your 0,0 point is. The next time you start ride your machine (jog) to this point......To get to the exact point I then change my motor tuning down to 50 steps...if you now jog with the arrow keys, you will move the gantry VERY slowly to reach your 0,0 mark....just remember to go back to your motor tuning and restore your NORMAL steps. Zero Mach3 on this point and you are ready to cut from the original0,0 point. Hope this helps

Hennie,

Didn't you install proximity switches? They make zeroing the table so easy.

Hi Nils, I suppose the proximity switches will always bring your machine to the same TABLE 0,0. How do you work with OFFSET's when your material is lying somewhere else on the table...I think this is the problem I don't understand how to adjust Mach3 to move from my table 0,0 to my current working piece 0,0....they could be different point's on the table.


I need to study Mach3 more to get to grips with it. I am sure it can be done easily,..just need to be shown / told first time...Monkey see Monkey do....works for me..Reading the manual....I am bad with that.

Kobus,

Look at the Offset Tab and then Active Work Offsets. You can set up I think it is 99 Work Offsets. Location on you table that you can goto once you have picked that offset. This enables you to have locations that you have a jig or material located that you cut the same file. No Brainer way to repeat jobs.

I would advise going through the Mach tutorial videos. I forget which one it is but it explains how to use them.

I have one set up so at the end of using my machine I run an offset to place the gantry in one spot.

The proximity switches are a safety precaution and they make zeroing the machine easy.

I hope that helps.

Hi Kobus,

You can always jog to your work piece, align your cutter at zero and then zero the axes at that point and then start your gcode.

Greg

Kobus, hard stops are just as good as proximity switches for zeroing the table. . . . . hold the gantry/car against the stops, switch on motors, zero the table. This done once a week or once a month, or after a power failure, or hitting a clamp. Jobs (with their fixtures) are zero'ed independently and Mach remembers their offset from the table zero (even after a power failure or hit clamp).

I have forgotten all the correct terminology and button names for Mach, but the main thing to get your your head around is that there is a table zero and up to 99 job zero's. The table zero is rarely displayed, but never forgotten. The two zero systems co-exist in parallel to each other.

How to line a tool up to a jig? Well, our jigs are mostly bits of scrap quickly screwed to the table.....then we trim the working faces of the jig and zero according to those last known cuts. The job butts against a fresh jig with a known cut position. In other words, we don't try to hover a pointer above the jig to try and sight a zero position.

Thanks for the advice will try it tomorrow.Nils I did buy the proxies but have not yet installed them had no time yet

I suppose there are many way's to skin a cat and many way's to set up the machine to cut from any point. My way is not using all the power of Mach3 to do things, but I found that with my manual way I am sure that I start my cut at the correct point. I don't have to calculate or remember offsets and therefore I have never cut into any clamps or any other objects. Someday I will check out the offset functions in Mach3 to see if I like it. Maybe I just afraid of trying to learn something new now that I have my cutting control under control with my manual way.

Kobus,
I have found sometimes the best way to do things is whatever you feel most comfortable with. Like you said, if you look into the offset features of Mach, then you might find a new way that makes more sense to you. I tend to use whatever makes the most sense to my twisted mentality. ;)

On the question of home switches, they work very well. While I battled with getting to grips with the CAM software, I actually restarted several jobs over and over. You just send the machine home and then apply the fixture that you saved in Mach. If you look at the 3D mould that I cut on the forum below, you will see two seperate moulds cut from the same piece of material. On the first mould I had to change the tool midway through the job because it was to short. I just homed the tool and continued the gcode at the line I left off. Was it not for the home swithes I would have to start from scratch.

http://www.mechmate.com/forums/showt...?t=1223&page=4

Sounds like you all have pretty much figured out how to accomplish this. I assume the reason this is an issue is because the steppers do not provide positional feedback, like a servo can...right? Forgive my ignorance on this issue as I'm still wading thru all the info. Surely there must be a way to provide positional feedback w/o too much effort....or is it really not a big deal in practice?

Chris, none of us agonize much about where to hook a tape measure. :)

Same with the machine - point it at a spot and tell it "this is zero".

Oh well that's easy enough...if all you need to do is to "tare" the system (which I assume you simply do thru your software) then that is a non-issue from what I can see.

Chris, positional feedback is not required on a stepper based system. Having a know starting point is however important if you are going to to repetitive work or complex cutting that might require that the job be restarted during a process. IE, I cut moulds for people that has to have multiple processes done during the manufacture of the mould. I would have to do some cutting and then remove the job for someone else to do some welding or coating or something. The job must then be replaced at the same spot. I use the home position of the machine as well as a fixture offset to recalibrate the tool position very accurately. If you are going to be cutting parts from some material, it does not really matter where you chose the zero position of the tool to be.

Check on the Mach3 offsets page (alt-5) you will find there work offsets from G54 to G59 and at the bottom right corner of that screen you will see a big button Save Work Offsets.

The procedure is like this:

Mach3 starts with G54 (unless you initialize it as other offset)
you reference all your axis using some of your limit switches as home (you have to configure this in homing and limits)
then you go to the offsets page and select the offset you want to use
bingo, the work 0,0,0 is where you programmed it.

You can even use different offsets in the same program, for example to repeat the same work at a different location (think about tiling your work)

Lots of choices!