Homing switches & 'methods of working' (Mach3)

[HankMcSpank]

Just fitted home switches to my machine & I’m now trying to figure out the best ‘methods of working’ with these in place!

When knocking up something in CAD/CAM, I base all my designs around the origin – eg if drawing a circle, the centre would be the ‘origin’ ….therefore before home switches, I’d simply jog my machine’s table to the centre of its axis travel then zero the coordinates….then I’d simply start the cycle.

But now, in Mach3 with home switches present, when I click ‘ref all home’ (btw: not sure if it relevant – but my table homes to the negative extremity of both X & Y axis), it then zeros all the axis…therefore if I load my Gcode, the lower part of the aforerementioned circle will not be ‘reachable’ by the machine.

One immediate solution is to establish the central point of my table, then offset my work at the end of the CAD/CAM process to reflect this for my GCode ...but is this how it's normally done?

If not,what should I be doing to ensuring that my machine works in the middle of it’s axis travel, yet still have the possibility of ‘homing’ should the steppers stall if I’ve pushed them too hard!

[ptjw7uk]

I have often wondered about the same thing as to my mind a homing switch should be in the middle of the travel and limit switches at the extremities. If a homing switch is in the middle then its construction will dictate how accurate the position will be depending which direction the position is reached from(if you get my drift! - no pun intended)
So far Ihavent fitted switches to my mill as I dont see how they are going to be that useful!

Peter

[HankMcSpank]

I have often wondered about the same thing as to my mind a homing switch should be in the middle of the travel and limit switches at the extremities. If a homing switch is in the middle then its construction will dictate how accurate the position will be depending which direction the position is reached from(if you get my drift! - no pun intended)
So far Ihavent fitted switches to my mill as I dont see how they are going to be that useful!

Peter

Hi Peter....there seems to be a problem with homing switches for the hobbyist - lots of sites tell you how to implement them (indeed it only took me about 45 mins from scratch to fit mine & get them working) & I can certainly see the *massive* win wrt pushing steppers too hard & them stalling, then losing your place - but there seems to be scant info about how such switches fit into the overall picture/workflow wrt using CNC machines!

I stumbled upon something via Google today that I need to investigate a little bit more - a possible 'offset' from the 'ref all home' position, which I can only assume means something along the lines of "after homing to a known point, go offset to position by Xx & Yy (ie the middle of your table) & then consider this to be 0,0. Something like that would make sense.

I'll update you if I suss this one out tonight!

[audioandy]

Hi Rob

Home switches are useful for repeatability if you want to use the center of the table you will use one of the offsets in Mach, G54 onwards I think they are, so you could set up a fixture in the center of the table then using the offset go to the exact same start position every time.

Hope that makes sense!

Andy

[John S]

Andy has it in one,
Read up in the Mach manual on the use of G54

[HankMcSpank]

Ok, this is one of those things that's just better to try out than explain! But the magic words in play were indeed offsets (I was looking for 'homing' related info earlier!)

Anyway, in Mach3 go to the 'offsets' screen & in the X & Y fields, enter the distance from 0,0 set by the homing switches (machine coord home) to the 'middle' of your table.

Now, when you click 'ref all home', your machine still returns to the homing switches, but now once the axis have homed rather than the DRO reading 0,0, they'll now read with whatever your entered offset is offset is (eg on mine when homed the DRO will read X -110, Y -60)

Now click on 'Goto Z' and your table will move rapidy to position 0,0 (which is the middle of your table)...you can load up your G-Code as normal knowing that you can get back to this point in an instant.

Lovely, I have exorcised the DIY CNC demons....no more worries about having to start from scratch if/when my steppers stall!

Thanks!


PS, Just one thing, apparently the offset settings are only a temp setting in Mach 3.....meaning they'll be lost each time you exit Mach3

To have your machines specific offsets load up everytime you start Mach3, a google search reveals the following workaround (& it might seem a load of old gobbledegook, but it's simple enough to follow with the screen in front of you - & it works)....

"On the offset screen, click "Save Offsets". Scroll down to the last one, G59P253. Set up your X & Y offsets there and save.

Open the General Configuration screen. At the bottom right side, check the box that says "copy G54 from G59.253 at startup". Restart Mach3 and you'll have your G54 offsets."

[Wobblybootie]

Thank you all, I am nowhere near ready to deal with the physical problem of limit switches (still amassing parts) but I do ponder things like that when I get 5 minuets of quiet time. The problem was clearly laid out and the solution was just as clearly explained. This forum is worth it's collective weight in gold.

[John S]

One thing with CNC is there are no real right or wrong ways, just different ways of doing things

Some people use limit switches as homing switches and then use G54 to go to the work zero.
Homing switches take you to MACHINE CO-ORDINATES then using G54 this takes you to WORK CO-ORDINATES which is usually the corner of the work or vise. Many newbies have a lot of trouble with differentiating between the two.

A simple way to start is to use the corner of the work / vise and set both co-ordinates to this point and not use homing, a ref all or goto home will then use this same point.

It's purely personnel choice.

One final note when drawing parts to be used in a vise, The normal way of drawing which dates back from the old manual drawing board days is to use the bottom left corner as 0,0. This then makes all dimensions / moves positive but a CNC doesn't have to worry about this.

If you make this point 0,0 then it puts, on a normal setup, the origin point on the edge of the moving jaw. Any differences in blank size will make all the parts different from it's true 0,0

If you use the top left as origin it then puts 0,0 at the end of the fixed jaw and every part will be identical regardless of blank size. Most CAD systems give you the option to move origins so no matter how you draw on the last save you can set this to top left.

.

[Wobblybootie]

Cheers John, that makes sense and logical really, just never saw it like that. Yet another nugget of information to be stowed away.

[reuben005]

Even i am doing the exct same thing, with the 2 limit switches on the min and the max end of the axis, and the home somewhere in the middle. Even i am using the Work offset option.

The only problem i am having is that when i click the "Ref all home" button, sometimes the tool is at the negative side of the home switch and it keeps going negative until it hits the limit switch and the machine shuts down. Now i have no way of telling the machine which side of the home switch the tool is.

so any views?

[C_Bubba]

Even i am doing the exct same thing, with the 2 limit switches on the min and the max end of the axis, and the home somewhere in the middle. Even i am using the Work offset option.

The only problem i am having is that when i click the "Ref all home" button, sometimes the tool is at the negative side of the home switch and it keeps going negative until it hits the limit switch and the machine shuts down. Now i have no way of telling the machine which side of the home switch the tool is.

so any views?

This is why you put the machine coordinate at one of the limits of the axis. That way the Machine will always home in the proper direction. From there, you set your offsets for the various fixtures as previously noted. Fixture offsets are your friend! When you make a setup, you have the option to "save" the offsets. Now if you have a crash, power failure etc. You can simply restart the machine, home it and load the offsets and your back in business with no additional setup time. Sure, it may take a few seconds longer to make the setup, but it only takes one time to see how useful this can be. (Don't ask how I know:})

[Jonathan]

2 years 8 months lather and the thread is resumed, that might be a record!

[Robin Hewitt]

so you could set up a fixture in the center of the table then using the offset go to the exact same start position every time.

Andy hit the nail on the head. Homing switches are useful if you are working with a fancy metal clamping jig bolted down at a known location on the machine bed.

I don't use MACH because as soon as you start working from G code you lose touch with the original drawing and cannot refer back to it when you want to align tool to metal.

I locate by circles on the drawing, circles with a zero thickness do not cut but I can still see them.

I pop the drawing on the screen and every circle has a little pick box dead centre. Left mouse button on a pick box moves the tool to the circle centre, right button sets the mill XY co-ordinates to the circle centre.

Drilling holes becomes a doddle on my mill/drill, alignment is all sorted at the drawing stage.

[audioandy]

Even i am doing the exct same thing, with the 2 limit switches on the min and the max end of the axis, and the home somewhere in the middle. Even i am using the Work offset option.

The only problem i am having is that when i click the "Ref all home" button, sometimes the tool is at the negative side of the home switch and it keeps going negative until it hits the limit switch and the machine shuts down. Now i have no way of telling the machine which side of the home switch the tool is.

so any views?

The only thing I can think of for a work around on this is at the end of your G code when your tool maybe goes to X0 Y0 Z30 (example only) you can change the code so your axis finish on the positive side of your home switch so X50 Y50 Z30 (example only) then when you reference you should be ok.
Other than that move your home switch to the Neg side of movement on your X and Y axis.

hope this helps

Andy

[motoxy]

I don't use MACH because as soon as you start working from G code you lose touch with the original drawing and cannot refer back to it when you want to align tool to metal.

I locate by circles on the drawing, circles with a zero thickness do not cut but I can still see them.

I pop the drawing on the screen and every circle has a little pick box dead centre. Left mouse button on a pick box moves the tool to the circle centre, right button sets the mill XY co-ordinates to the circle centre.

Drilling holes becomes a doddle on my mill/drill, alignment is all sorted at the drawing stage.

May I ask what you use if you do not use g code?

bruce

[Robin Hewitt]

May I ask what you use if you do not use g code?

You only need G code to transfer the cut from the program that produced it to the program that does the cutting.

My software creates the cut then pumps it directly to the mill so I miss the file copying stage, no need for G code.

Having the original drawing as well as the cut available makes setting the mill a doddle, but I can't say I'd recommend it :very_drunk: