Setting up soft limits in UCCNC .. "Logic"

[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.

[John11668]

I never really expected this post to give rise to so much controversy.
I was really just looking to get clear in my head what settings to put in there.
I think I have achieved that, but it has become clear that different users operate these in a way which suits their own purposes.
At least I now know how I intend to operate in order to have a method which suits me .

Thanks Guys.

[JAZZCNC]

I never really expected this post to give rise to so much controversy.
I was really just looking to get clear in my head what settings to put in there.
I think I have achieved that, but it has become clear that different users operate these in a way which suits their own purposes.
At least I now know how I intend to operate in order to have a method which suits me .

Thanks Guys.

This isn't controversy John just friendly banter just wait until we really get fired up...

We all use our machines in different ways with different setups and their is no right or wrong way. Plus I guarantee in a years time you'll be doing it a completely different way to now as you learn and advance more.!

[Neale]

John - one of the difficulties here is that there is a bit of an onion skin effect - it looks simple from the outside, but each time you peel off a layer of understanding, there is another layer of complexity beneath! I don't think that there is any particular disagreement between any of those who have posted, but we each tend to have our own way of looking at things. For example, Kit mentioned woodworking gantry machines and mills as if they are different. Well, of course they are mechanically, but in terms of machine and work coordinates they work exactly the same way. But the complication comes when you watch them at work - in the first case, the tool moves around the work, in the second the tool stays still and the work moves! The only thing that matters is the RELATIVE movement between work and tool, and that is (or should be set up to be) the same in both cases.

Couple of things that have been mentioned. G54, G55, etc - these refer to different work coordinate systems. The motion control software notes the offset between machine and work zeroes when you set them up. It can save these values, so that when you come back to the machine it remembers the offsets and, once you have rehomed the machine, your work zero will be in the same place as before. Sometimes it's useful to have several work coordinate systems, if you have some jigs and fixtures on the machine, for instance. So you can set work zero for each of these, and save them as the G54 (the usual default set), or G55, or G56, etc. Then in your gcode, it will tell the machine which set to use for a particular fixture, say, and you don't need to reset each time.

Jazz also mentioned the "backing off" feature. I'm with him on this - as mentioned a few posts ago, there is no reason to have the machine zero anywhere except in the "bottom lefthand" corner, but you might want to use the opposite end of machine travel for your home position. A friend of mine has his router set up like this - this commercial machine has the home switch at the +X end of the bed, so it homes to there but effectively sets the machine coordinate zero to correspond to the -X end of the bed. However (and I have exactly this problem on my own machine) you can sometimes get a problem when homing. For example, I home X, and by default the machine then leaves X where it is and starts homing Y. But the tiny vibration that is caused trips the X switch which then gives a limit error. Pain in the neck! The answer is to use the backoff feature to move the X position a milllimetre or two off the switch and set zero there. Then there is no accidental switch triggering and homing becomes reliable again.

These discussions come up every so often but it's worth airing because this is a big stumbling block when you first start out. Give it month or two of use and you'll forget you ever had a problem, but it's a real brain-strainer at first!

[John11668]

I think I am getting it Neale and I must admit I had never considered the Gantry machines.
I did work with NC gantry routers in the aircraft industry in early 70s milling Jaguar wing skins complete with pockets, ribs and stringers. A 70mm slab roughly the size and shape of the wing, was held on the table by Vacuum while most of it was machined away. One man "operated" the machine . Or really he watched it .
Three others removed barrowloads of swarf to the skip in the yard and they really did have to work.

In those days the machines were tape driven and " wizards" came in from elsewhere to set the machines up. CNC was spoken of in hushed voices as a black art.

Quite a few topics have been covered in this thread above , which really have served to reduce the mystery a tad, so now I can go and play a bit and make sure I have grasped the principles .

Thanks to all !

John

[Kitwn]

Clive, Dean,
Thanks for the links and comments.

I've never really thought about being able to save a variety of offsets in the software, though I have been known to use a carbon based data input interface and non-volatile planar organic storage medium to record them in the past. As I'm now starting to use a couple of different jigs for streamlining work, that may be more sensible.