Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: rabphxaz on December 25, 2008, 08:22:43 PM
-
I was trying to run a test prior to cutting my first piece and I realize that I don't understand HOME. I figured I would design a small 3" x 5" rectangle, jog to the middle of the table and run the file in the air w/out the router on, but when I got there and tried to change the X, Y, and Z absolute home zero to that new location, I couldn't do it. I first clicked Machine Coordinates, then zeroed the axes, then clicked Ref All Home, but the Abnormal Condition light started blinking and when I checked the Diagnostics Page I found that the old home position hadn't changed. What should I have done?
Also, whenever I close Mach 3 I get a Fixture Save? query, even when I haven't loaded a Gcode file. What kind of fixture are they referring to?
Thanks again, Bob
-
Bob,
If your machine does not have home switches, you don't need to concern yourself with the whole concept of home - It's of no value to you. Decide where you want zero to be for the job you're running, put the machine there, and zero the user coordinates. Don't worry about what the machine coordinates are, they're not important.
Home is only useful if you have home switches, and it's primarily useful for quickly re-zeroing the machine after power-loss, a tool-breaking, etc. Without home switches, you just have to manually re-zero to whatever you chose as your user coordinate zero point if something goes wrong.
Regards,
Ray L.
-
Oh, on the second question - it's asking if you want to save the offsets for the fixtures defined by G54-G59, etc. Again, without home switches, there's really no reason for you to care. Save them. Don't save them. Doesn't really matter.
Regards,
Ray L.
-
Thanks again, Ray, and Merry Christmas.
All the best, Bob
-
Bob -
The machine needs to know where it is before it starts. It keeps it's position in Program Co-ordinates which are displayed when the program co-ordinates led is lit. To this it adds all the various offsets for programs and tools etc, so the tool arrives at the right place at the right time.
On commercial machines, the first job of the day is to "home" the machine - done in Mach by selecting the various home switches. The machine will move to a position that it knows is 0.0.0 in machine co-ordinates and set the DRO's accordingley. It is now "home" . The home position is probably not any good for machining from, and will certainly not bear any relationship to the 0.0.0 position the program is written from - so each program then has an "offset" written into it, which brings the machine to the correct position to start work on that program.
If you do not have home switches fitted and activated, Mach has been written so that your machine co-ordinates will zero at any position.
You should, therefore, move your machine to a suitable position to start your program, and this is normally (but not necesarily) the 0.0.0 position of the program you are about to run.
The safest way to proceed is then to press "machine co-ordinates" so the button is lit. The machine is now displaying "machine co-ordinates" and then press "RefAllHome" This will zero the machine co-ordinates. Then press the "machine co-ordinates" again, the led should go out. The DRO will display "program co-ordinates" This could be 0.0.0 or could be a random set of numbers from your last job.
Zero each DRO using the zeroX, zeroY and zeroZ - the DROshould again display all zero.
You now have the Machine Co-ordinates and the Program Co-ordinates all singing from the same hymn sheet, and you can start your program run.
Why so much fuss - if you do not have both sets of co-ordinates in a fixed relationship to each other (here they are identical - which is the simplest relationship - i.e. the offset is 0.0.0) then any offsets in your program will not necessarily work correcty, and you will be left wondering why.
There is nothing wrong with starting like this, I have home switches on my lathe, but for some "one-off" jobs, it is easier just to get on with it rather that worry about all the offsets using the homing switches. Fitting home switches is something you can tackle later - if you feel then need to do so.
If you look under Config/Fixtures you will see a fixture table. This has from G54 to G58 then another 250 or so from G59P7 upwards, which allows you write a lot of programs, each with it's own start point. If you were in a long run, and closed overnight, when you came in the morning you would zero your machine and press "GO". The machine would pcik up the offset from the fixture table, move to the correct position for that program and get on with it, without further ado. Some porgrams have the same series of instructions, working from different "offsets" if cutting say, patterns out of a large area of material.
These offsets mgiht change during the day, so when Mach shuts down, it saves all the current fixture list, so it is ready for the next day.
-
Jimpinder,
Very good write up ( as usual ) with the why part included. One worth saving. :)
RICH
-
...if you do not have both sets of co-ordinates in a fixed relationship to each other (here they are identical - which is the simplest relationship - i.e. the offset is 0.0.0) then any offsets in your program will not necessarily work correcty, and you will be left wondering why....
If you don't have home switches, under what circumstances will it matter what the machine coordinates are? You shouldn't be running any G-code that cares....
Regards,
Ray L.
-
Ray - Yes you are right, and I could not think of circumstances where you would use offsets., but never-the-less I feel it is a good idea to understand the relationship between machine and program co-ordinates, when it comes to using them.
You could, of course, make your own "home" without having switches fitted - i.e. a place where you can put the table with some repeatable accuracy - and then zero the machine co-ordinates.
I must admit, I am in a quandry on the lathe. I home my machine - but where then to move to. x axis is down the centre - that is easy, but the z axis ???
Do I have 0 position at the chuck - (if so is it right at the chuck, or about 10 mm off, so a parting tool can get in behind), or is it at the opposite end of the workpiece. That one I will have to ponder.
At least the X axis is fine, and my centre drilling fixture works a treat.
Dom't worry Bob, just an old man ruminating at Christmas - and the best to you all in the New Year.
-
Jim
for the lathe I would say home position of X fully away from the centre would be a better option. Z is a trickier proposition if you have a tailstock.
It could be argued that a Z home is not really needed as you mostly zero to the stock end but I have one on mine as it was there and I do use it.
My X axis is actually not fully away from the centre in the conventional respect as I have both front and rear toolposts so if it was then the front post would be at centre, instead mine is positioned so that both front post and rear turret are equal distance from the centre.
My Z axis home switch is moveable so if I wish I can have a home at any position but I tend to just have it in a fixed location.
The major benedit to having home switches is so that you can also set up softlimits but for a lathe softlimits are really not much use as you can have tools sticking out in all directions and thus could smack one into a chuck and still be well within the axis limits.
Hood
-
Hi All,
I don't have any limit switches on my mill but may add them someday. Attached is a file which describes
setting up homing without limit switches and may be of value if someone wants to fool around some.
RICH
-
As usual, the forum community comes through with excellent information, and I thank you all once again. Here are 2 more questions that I am now at the point of dealing with:
1.) Suppose I want to route out a flat, level area that is in the shape of, say, a star, in flat material, and I want to have fairly sharp corners. I will use the offset tool set for a 1/8th inch end mill bit, which will give me satisfactorily sharp points on the star. But the star is large, and I don't want to have to route the whole thing with a 1/8th inch bit. How do I write the program to allow for a tool change to a, say, 1/2 inch end mill?
2.)I have used a 1/8th inch end mill to define a work area on my table by drilling down into the table with the bit at the 4 corners of the work rectangle. I have zeroed the xy to the lower left corner of that rectangle by setting the zeroes at the place where I drilled that hole. I then drew lines on the table that touch the outside edges of each 1/8th inch hole. Should I change the xy zero locations to account for the center of the bit being 1/16th of an inch from the line? Will the software know to offset from that 00 location when I change bit sizes?
Thanks again, and Happy Holidays to All,
Bob
-
Hood -
Yes, like you, my x axis homes between my front tool holder and my drill holder. Following your advice, all my drills are in holders and the tool offsets set so that selecting the tool, then Z0 and then X0 brings the tool to a position on the centreline and 5mm from the chuck.
I have done a similar thing with the cutting tools.
I finally decided on 5mm from the chuck as my Z0 because it allows a parting tool between it and the chuck, and it is an easy figure to remember when designing things. Ball screws now - so had to go metric.
Bob -
Offsets for milling tools and diameter compensation have been covered many times, but the best one was by Graham Waterworth a few months ago, with diagrams as to which command to use depending on the way you were cutting. Try and look that up, becasue Graham is the man for that sort of thing.
I am not competant enough to advise, although - yes - you can use different sized cutters, and the same program, the compensation will automatically adjust for the width of the cutter. You have a problem with lead in and lead out.
I am wondering if it would be better just to design the star, using the bigger cutter, and writing the Code for the toolpath, then changing the tool and writing code for the toolpath to cut the sharp points, if you see what I mean, and make allowances in the code for the cutter width.
On your second query, your zeroing of the axis was not accurate, because the line you drew was outside the centre points of the bit so your actual 0.0 position is minus 1/16th on each axis, if you are lining up to the lines you drew.
I don't know how many stars you are cutting, but you can now see the benefit of "home" switches. If you can "home" your machine (and the actual position does not matter) then a simple offset G54 - G59 written into the program will always bring the table to the correct position for that program. You only have to set up once ;D
-
Ball screws now - so had to go metric.
Ha ha , well supppose you had to come into the modern world at some point in time :)
Hood