Setting up soft limits in UCCNC .. "Logic"

[Neale]

I'm a bit concerned that anyone thinks that "going past zero" is in any way relevant when you are using Mach3/UCCNC. Maybe in the days of archaic controllers that did not have any homing/work offset capability this might have mattered but not today.

The point here is that homing sets machine zero, either directly by putting home switches at the zero point, or somewhere else with an appropriate offset (at the right-hand end of travel, in the most extreme case). But that is absolutely nothing to do with where the zero point is on the work. First thing you do when you plonk the stock on the bed and clamp (assuming that you have already homed the machine) is to move the spindle to where you want (0,0) to be, and then set "work coordinate zero" to that point. Maybe x and y at the same time, maybe separately. Effectively you are doing the same thing when you set tool height - this is setting z coordinate zero, indirectly. Your gcode will, if generated by any modern CAM package, be working in terms of work coordinates. Nothing at all to do with machine coordinates. For example, recently, I have been machining work where the X zero work coordinate is at the right hand side and most of the machining is done with negative X coordinates. I told my CAM software where I wanted X=0, set the spindle to the RH edge of the stock and set work coord X to zero, and away it all went.

This machine/work coordinate confusion is a bit complicated to follow at first sight but it soon becomes second nature and you won't even think about it, but it is absolutely critical to using CAM and the machine in harmony. I sorry if I have misunderstood what was being said, but the idea that you need to set machine zero somewhere on to the bed just so that you can move to negative coordinates could be very misleading to anyone new coming to this.

[John11668]

I'm a bit concerned that anyone thinks that "going past zero" is in any way relevant when you are using Mach3/UCCNC. Maybe in the days of archaic controllers that did not have any homing/work offset capability this might have mattered but not today.

The point here is that homing sets machine zero, either directly by putting home switches at the zero point, or somewhere else with an appropriate offset (at the right-hand end of travel, in the most extreme case). But that is absolutely nothing to do with where the zero point is on the work. First thing you do when you plonk the stock on the bed and clamp (assuming that you have already homed the machine) is to move the spindle to where you want (0,0) to be, and then set "work coordinate zero" to that point. Maybe x and y at the same time, maybe separately. Effectively you are doing the same thing when you set tool height - this is setting z coordinate zero, indirectly. Your gcode will, if generated by any modern CAM package, be working in terms of work coordinates. Nothing at all to do with machine coordinates. For example, recently, I have been machining work where the X zero work coordinate is at the right hand side and most of the machining is done with negative X coordinates. I told my CAM software where I wanted X=0, set the spindle to the RH edge of the stock and set work coord X to zero, and away it all went.

This machine/work coordinate confusion is a bit complicated to follow at first sight but it soon becomes second nature and you won't even think about it, but it is absolutely critical to using CAM and the machine in harmony. I sorry if I have misunderstood what was being said, but the idea that you need to set machine zero somewhere on to the bed just so that you can move to negative coordinates could be very misleading to anyone new coming to this.

As you say Neale it is not at all intuitive to begin with, and I dont believe I have seen a clear explanation in the manuals . ( and some of the videos are even less helpful)
I think I have got it now though.
So by homing and setting soft limits you are defining the extremities of the working area, within which you will place your job.
You then choose a point on your workpiece which you will define as 0,0,0 for you starting point, traverse your tool to that point and you will then set the work coordinates to zero on all axes.
The G code routine will then move the tool in whatever positive or negative directions are needed to complete the work.

I suppose it becomes particularly clear when doing say an engraving job where conventionally you will set z=0 when the tool is touching the surface, then any movement to Z negative involves a cutting depth and movement to Z positive gives a clearance for tool repositioning.

[JAZZCNC]

I'm a bit concerned that anyone thinks that "going past zero" is in any way relevant when you are using Mach3/UCCNC. Maybe in the days of archaic controllers that did not have any homing/work offset capability, this might have mattered but not today.

The Problem here Neale is that word HOME confuses people. They mix it up with WORK ZERO and think that HOME is where the JOB starts.
99% of new users fall foul of this so when I deliver machines to new users I always spend at least 30mins or more explaining and showing how the COORDINATE SYSTEM's and WORK OFFSETS relate to each other and how they relate to CAD etc.

Now John11668: and anyone else who doesn't quite understand. This is where SOFT LIMITS can come into play to save the day.? Let us say your HOME (machine zero)position is at the end of travels on each axis and you have 1000mm of travel.

You ZERO the WORK coordinate 100mm from the MACHINE ZERO. The job is drilling holes in a 1000mm long piece of stock with the last hole located 990mm from 0. What do think will happen .?.....Yep CRASH.!! . . Because your last hole would actually be located 1090mm from MACHINE ZERO. . . . But not if you have SOFTLIMTS turned on because the controller will pre-run through the G-code when you first load it and will warn you that you are going to exceed the SOFT LIMITS and the day is saved...

So hopefully this shows how MACHINE ZERO and WORK OFFSETS play together.

[John11668]

Hi Jazz and thanks for your response .
I dont think however you have quite clarified things for me.
So ignoring backoff for now .
I home to machine zero in all axes and the machine defines its position as 0,0,0
I have set soft limits X of 0 and 400.
Soft limits Y of 0 and 200,
and Soft limits Z of 0 and -50
So I have now defined a box 400x 200 x50 which is the envelope within which all work MUST be done .

We now come to the workpiece which I have to plant on the table completely within that envelope and clamp it. I have to bear in mind if I am doing an outside profile that I must consider the cutter and allow at least a cutter radius all round.

I am guessing that my workpiece origin or start point is defined somewhere within it , whether it is right hand end, middle, or wherever so I identify that origin, jog to it , and set all my work parameters to zero at that point.

So really it is only if I have placed my job wrongly and that the toolpath will stray outside the envelope that a soft limits alarm should arise .
Are you saying that it should arise prior to hitting the start button . or will it only arise when the work zero position is defined .

[JAZZCNC]

So really it is only if I have placed my job wrongly and that the toolpath will stray outside the envelope that a soft limits alarm should arise .
Are you saying that it should arise prior to hitting the start button . or will it only arise when the work zero position is defined .

Ok lets say you define your WORK ZERO in X half way up the work envelope (or put another way 200 in MACHINE coordinates.) And you defined the X ZERO point in CAD to be bottom left corner of the part and the part is 400mm long in X. When you load the code and it does it's Pre-check it should warn you, I don't think it does when you push cycle start the control should warn you before then. (In UCCNC this feature might need turning on in the settings, I think it's called Softlimits pre check)

It's easy to test just set WORK ZERO for X & Y up the top so the part falls outside the cutting area and set you Z axis at the top of travel so no damage can be done if it it doesn't work but you'll know straight away because it shouldn't work at all in which case hit the stop button.

[Kitwn]

I'm a bit concerned that anyone thinks that "going past zero" is in any way relevant when you are using Mach3/UCCNC. Maybe in the days of archaic controllers that did not have any homing/work offset capability this might have mattered but not today.

The point here is that homing sets machine zero, either directly by putting home switches at the zero point, or somewhere else with an appropriate offset (at the right-hand end of travel, in the most extreme case). But that is absolutely nothing to do with where the zero point is on the work. First thing you do when you plonk the stock on the bed and clamp (assuming that you have already homed the machine) is to move the spindle to where you want (0,0) to be, and then set "work coordinate zero" to that point. Maybe x and y at the same time, maybe separately. Effectively you are doing the same thing when you set tool height - this is setting z coordinate zero, indirectly. Your gcode will, if generated by any modern CAM package, be working in terms of work coordinates. Nothing at all to do with machine coordinates. For example, recently, I have been machining work where the X zero work coordinate is at the right hand side and most of the machining is done with negative X coordinates. I told my CAM software where I wanted X=0, set the spindle to the RH edge of the stock and set work coord X to zero, and away it all went.

This machine/work coordinate confusion is a bit complicated to follow at first sight but it soon becomes second nature and you won't even think about it, but it is absolutely critical to using CAM and the machine in harmony. I sorry if I have misunderstood what was being said, but the idea that you need to set machine zero somewhere on to the bed just so that you can move to negative coordinates could be very misleading to anyone new coming to this.

Neale,
I'm not going to argue with a word of this, and I am coming at it from a wood-working gantry router perspective which is different to a mill. Like you I often reposition the work coordinate zero to suit the job but this will be a known position relative to the homed (0,0) position so that it can easily be re-acquired after an E-stop or other driver-disabling event.

The OP was confused regarding numbers to put into these values but the main points I wanted to make are the need to pull away from the switches to a specified point after hitting them, (0,0) being the obvious label to put on that point in my view, and that the area the workpiece can fit inside will often need to be smaller than the area defined by the soft limits which primarily exist to prevent crashes but also specify the limits of movement of the centre of the cutting tool. The best numbers to use then fall out from there.

Kit

[JAZZCNC]

Neale,
I'm not going to argue with a word of this, and I am coming at it from a wood-working gantry router perspective which is different to a mill. Like you I often reposition the work coordinate zero to suit the job but this will be a known position relative to the homed (0,0) position so that it can easily be re-acquired after an E-stop or other driver-disabling event.

Kit, you don't need to position the work to a known MACHINE location to get back to WORK ZERO that is the point of the G54, G55,etc WORK OFFSETS and using HOME switches. If you get lost or crash the machine you simply HOME the machine and it uses the WORK OFFSET to get back to WORK ZERO.

The only thing you may need to do is save the WORK OFFSET before starting the job just in case power goes off mid job. However some controllers save the WORKOFFSET before the start of the job, I think Linux does this and UCCNC but Mach3 doesn't which is a pain as it's easy to forget.

Regards Backing off the HOME switch then the only point to me, other than to relocate MACHINE ZERO position is to stop potential false trips if using same switch has limits combined with homing or to square a dual motor gantry.

[Kitwn]

Regards Backing off the HOME switch then the only point to me, other than to relocate MACHINE ZERO position is to stop potential false trips if using same switch has limits combined with homing or to square a dual motor gantry.

A precise and detailed description of my own machine!

I love threads like this, I always learn a great deal myself and as I discovered when I took up teaching technical stuff to adults back in the 80s, there's nothing will show up the holes in your own knowledge more effectively (brutally at times!) than trying to explain things to someone else. I now need to swot up on the full details of G54, G55 and other relevant codes and exactly how LinuxCNC uses and saves them.

The difference between machine coordinates and work coordinates is, as Neale pointed out, a confusing one tro begin with but soon becomes one of those fundamental bits of knowledge you don't realise you never knew.

[Clive S]

. I now need to swot up on the full details of G54, G55 and other relevant codes and exactly how LinuxCNC uses and saves them.

Yes this confuses many people. Have you noticed that you can see the machine coordinates and the current G54,55 etc on some GUIs at the same time. In Linuxcnc you can turn them on and off from the view tab.

Ie. If you have touched off your part ie X0,Y0 in G54 you will see the machine G53 at the same time completely different.

http://linuxcnc.org/docs/2.8/html/gc...es/offsets.png

http://linuxcnc.org/docs/2.8/html/gc...ordinates.html

[JAZZCNC]

I now need to swot up on the full details of G54, G55 and other relevant codes and exactly how LinuxCNC uses and saves them.

Probably without knowing it you and many others have actually been using a WORK OFFSET in fact if you have been using 2. These being G53 and G54.

When you HOME your setting G53 ZERO which is MACHINE coordinate system and when you set WORK ZERO you're using G54 WORK OFFSET. Almost all controllers, Mach3, UCCNC, LinuxCnc, even industrial-grade controllers like Fanuc, etc use G54 by default and unless you specifically need to use a different OFFSET say for things like multiple vises with OP1 OP2 type setup or several Fixture Jigs which all have a ZERO point you don't need to know about them.

Most CAM packages are also set up to use G54 by default which is another reason why many users don't actually know they are using WORK OFFSETS.

If you have a large working area WORK OFFSETS makes cutting several different jobs say as in different materials or thickness very easy because of each Fixture as it's own ZERO.