[777funk]

I just picked up a 040 machine.

I'm about to start using it but have run into some problems.

1. I would like to have a set in stone... EVERY time, never gonna change, home point. This way I can be sure that my fixturing jigs will always line up to the table and to my CAM outputs every time I run the program. It seems like home on my machine using Techno GCode is just wherever I last Zeroed the machine. In other words it can change. This could lead to big problems if the computer looses it's software or I have to reinstall on a new computer. All my fixturing jigs would be trash and I'd have to start over. I want to make sure that there's a ZERO point that I can rely on every time (i.e. set in stone). Is this possible?

2. I'm having a slightly hard time getting the CAM software to have it's start point line up at the same starting point as the machine (I guess the origin or home maybe?) Right now when I output things are turned or even trying to cut off the machines table (i.e. it's sending the machine past it's boundary and timing out). The scale looks to be correct but I am trying to get the origins to match up and having trouble. Is there an easy way to do this?

thanks!

[RandK]

Home is set by microswitches on each axis and is fairly repeatable. This is fixed, nothing you do will change that. After being powered on the machine won't do some things until you home so it knows where it is.

Your origin (zero point of each axis) is whatever you set it to. You could set it to home, or to any location within the travels that is a fixed offset away from home, which it sounds like what you want. You do this by setting offsets in setup, where you define the distance offset from home that you wish your zero to be.

If you just powered it up:

1. Home all
2. Zero all
3. Setup>offsets select your offset to use (this will zero again where you want it)
4. Touch off your Z for the bit and stock you want to use

One you decide where you want to place fixtures etc on the table and make your offsets you can make a reference drawing (rectangle) in a layer that shows where your table travels are in relation to your origin. This way you can check to make sure you are not exceeding your travels in locating your parts.

For my 054 I have my origin set a few inches north of front and center to make it easy to reach things. This means my part will only be machined in the positive Y direction but both positive and negative for X. It's totally up to you, but you need to match cad space with where you've set your offset/origin.

[777funk]

Home is set by microswitches on each axis and is fairly repeatable. This is fixed, nothing you do will change that. After being powered on the machine won't do some things until you home so it knows where it is.

Your origin (zero point of each axis) is whatever you set it to. You could set it to home, or to any location within the travels that is a fixed offset away from home, which it sounds like what you want. You do this by setting offsets in setup, where you define the distance offset from home that you wish your zero to be.

If you just powered it up:

1. Home all
2. Zero all
3. Setup>offsets select your offset to use (this will zero again where you want it)
4. Touch off your Z for the bit and stock you want to use

One you decide where you want to place fixtures etc on the table and make your offsets you can make a reference drawing (rectangle) in a layer that shows where your table travels are in relation to your origin. This way you can check to make sure you are not exceeding your travels in locating your parts.

For my 054 I have my origin set a few inches north of front and center to make it easy to reach things. This means my part will only be machined in the positive Y direction but both positive and negative for X. It's totally up to you, but you need to match cad space with where you've set your offset/origin.

So if I ZERO the machine, that's where it's going to start right? If I somehow loose the computer controlling the CNC's controller box, I'd assume all of my settings in the software (my Zero points for X and Y) will be gone?

Is there a way to make sure I can preserve these points in actual data to make sure I can repeat it if/when I have to replace the computer and re-install the controller software?

I'm assuming from what you said that Z is Zeroed every time I chose to do so for a new material height (top of the material just touching the bottom of the cutter). And I'm also interpreting from what you mentioned and the manual that I can set the offset for X and Y for the auto homing function. So ZERO and HOME are two different things, is that correct?

[RandK]

Home is always the same place because it is set by bumping each axis into the mechanical home switch. It's pretty accurate and repeatable no matter if you power it down etc. But it's a mechanical switch and isn't really intended to be 100% accurate, so if absolute tolerance is needed, checking your location against reference features in your fixture plates would be a good idea.

Zero is always totally relative. If you use an offset setting then you lock in the relationship between home and where you'd like zero to be for that particular offset (you can have a bunch of them). A lot of people with routers just place their stock and then zero based on a corner or a location they'd like to start at. If you are using fixtures that hold the stock in predetermined locations you want to use work offsets.

Where your CAM program does things depends on how you have it placed in your CAD/CAM software. I think it is normal to have your datum or zero reference in the lower left corner of the stock. For guitar work, where your stock may have a center seam that is important to locate accurately, a zero setting for the X axis on the centerline in both cad space and on the table would work better. But it's totally up to you and you can pick and choose based on what you are making.

The controller software will remember the offsets if you change computers, assuming you transfer the files over.

Offsets also save the Z offset from home but this isn't very useful if you are manually changing tools (lengths) in the spindle/router. Best to get in the habit of touching off after changing an active offset.

[Montabelli]

home is where the machine goes when you tell it to home, in my experience relying on the accuracy of the mechanical home position is a folly I can't afford. it is subject to changes, and at times other mystical influences which defy logic.

0,0,0 is the reference point which relates to the drawing and there fore the g-code, and thus is what you need to keep in mind. I use shop built jigs to hold different jobs and there for I have reference points or pockets if you will, of known relative position on the jig so that which ever machine I set up on, I can set my machine to the exact position of that pocket and then it is in the correct relationship top the geometry to the origin , 0,0,0.

some fellows like to place the origin in the middle of the part, others pick someplace else. I like to have it in the lower left point of the screen in my drawings and I set my machine in the +1 orientation so the visual reference is the same when standing along the side of the machine. there is no one right way there is only the way that works best for you.

[jmb]

The switches we use for homing tend to be accurate to 4 mills. That's the worst we've seen testing here, though it depends on factors like homing speed, temperature, etc. So if you want an exactly perfect home position, you have to turn on the index homing feature for the axes you want perfect homing on (typically X and Y). This causes the homing routine to hit the switches and then back off to an absolute encoder position (called the 'index pulse'), guaranteeing a perfect home.

Go to Setup > Advanced > Homing Params. For M1 and M2, check the Index checkboxes.

When you do that, the software throws a big scary warning, because your machine might have a configuration that causes this method to fail. The idea here is that your switches have a "repeatability window" and if the absolute encoder position is within this window, sometimes the home position will be perfect, and sometimes it will be exactly one revolution of the motor away. This is a terrible situation, because tool holders and fixture positions are all related to this home position. If you're off by a full motor revolution, tool holder positions (and everything else) will be wrong and who knows what kind of things you'll break?

Luckily, version 1.421 (and a few previous versions too) of the control software checks to make sure you're nowhere close to the repeatability window. If you EVER get an error message saying that you're within the repeatability of the limit switches, take the belt off the axis, rotate the motor pulley a half-turn or so, and put the belt back on. And then re-home. Don't ignore the error.

Well, don't ignore any error. But especially not this one.

James
Techno CNC
Engineering

[777funk]

This is a little scary. So as far as home, the mechanical home (home to switch bump and jogging back the set distance) is accurate to .0004". I think that's what I read in the manual. But if it's subject to temperature etc... that's scary. I guess even if I'm within a few thousandths I'm probably ok. But what if it goes beyond that. That would mean start over time for my fixtures. That's not good.

Do you think I should be accurate to .002-.003" with the switch bumping mechanical home considering the environmental factors that you mention?

[Montabelli]

none of it should be scary, my experience is over the course of 18 years with the same machine, lots of changes failures fixes and replaced encoders, motors etc. what accuracy level do you need to maintain, and repeatability is probably more important than homing accuracy.

[777funk]

repeatability is definitely what I'm after with this. I'd like to make one set of fixtures for each part that I'm making, put it on location on the table run the part; switch the fixture, run the next part and repeat for several years. If something goes wrong with the computer, I'd like to have the same home base for the machine within a few thousandths somehow on the new computer. Basically if it's not the same reference point every time I'll have to make new fixtures regularly which I'm trying to avoid.

This is somewhat new to me and I'm wanting to know what I should expect. Thanks for the notes on your experience everyone.

[Montabelli]

if it's not the same reference point every time I'll have to make new fixtures regularly which I'm trying to avoid.

that is the point of the target hole in each form with a known location which is marked on the jig. one of the nice features of the techno software is it will allow you to jog to a specific point drop into a hole and adjust should your jig be slightly off, for whatever reason. it also serves as a double check, you pull down the go to menu and put in the x,y coords slow your jog and see if your cutter slides perfectly into the hole. if it does you have verified your position, if it doesn't move it so it does and reset your coordinates. it works for me, and it allows jigs to be set up on more than one machine.

[RandK]

James - thanks for explaining the index feature. So if I turn that on, I assume that home will now be in a new location than it was. If I correct my offsets by the difference then I should back to the same fixture datum right ? I have the older direct style motors (no belts) so if I get the message I need to remove the motor and spin the coupler on the ballscrew end ?

777funk - Not sure how you are planning to precisely locate your various fixtures so they are always in the same place on the table. Using a master fixture base with dowels or keys would help for that. If you ie profile the outside of your fixtures to some even increment of an inch size then it would be easy to use an edge finder to check your positioning against what you think it should be. Montabelli is describing using holes and pockets. Maybe you should test your machine by making a test fixture and running through everything until you are satisfied that you know what to do for your real fixtures.

[jmb]

RandK:
Yes, turning on Index requires that you reset your offsets (and tool stand locations). It's probably easiest to just redo the offsets rather than adjust the fixture itself, but either way will work. If you get the error message, you'll want to take the motor off and turn the motor shaft, not the ball-screw shaft (which is true whether or not you have a belt).

[RandK]

I'll play around with the index feature when I can. I'm running 421.21 and the offset screen table entry/edit doesn't work right. I can't double click to select the contents of a cell, can't use the positioning (arrows, home etc), can't see the cursor etc. The offset name field seems to be center justified and without the positioning I can't see what I've got. Have I got a bad installation, missing font or something, or are the tables messed up in this version. How to fix ? Thanks

[jmb]

The Offsets feature took a second for me to figure out too. If you want to edit a line manually, click the box (say, the Y 1 box), and press Backspace to clear the number. Then type whatever number you want.

In order to use a line, you have to double-click the cell in the USE column. It's the second one from the right. Then click the Use button.

To save the current position, click Store Current Position and type in the row you want to save it in.

[RandK]

It worked properly in 377 and doesn't in 421. I used to be able to double click to select and replace the value of a field, use the navigation keys to set my position within a field, and I could read the name field which I can no longer do since it's center justified and my names are longer than will display in the box and it won't scroll so I can read them. These are things that work in other areas of the program and no longer do in the offsets and tools screens. Is there something else I should do to report this problem ? Thanks

[Pplug]

Go to:

Feedback | TechnoCNC Router Software

And fill out the form with your problem and they will help you. They did for me. I received an email back the next day with all my questions and complaints answered.

[jmb]

Ooh, I see. The interface originally allowed you to only have 10 offsets. People complained, so we increased the number dramatically by doing it the way you see in 1.421. So functionally it's better, but I do see the annoying factor.

We've got a lot on our plate now, but I'll let you know if we add a good solution to the next release. Your install isn't broken.

[Rick Turner]

We use the left front corner of the phenolic vacuum table as our "XY" origin and occasionally check it to make sure it's spot on. We also installed a grid of 30 drill bushings in the table to use as absolute known alignment positions for our vacuum fixtures. This allows us to use bullet nosed fixreture dowels, two per fixture that mate with bushings in the underside of the fixtures. Basically, the first layer of any CAD drawing becomes the table and it's drill bushing locations, then the fixture, then the part. Works great, and the XY 00 is always the same...that corner of the vacuum table...no matter where the fixture is.

[Dave's_Not_Here]

We use the left front corner of the phenolic vacuum table as our "XY" origin and occasionally check it to make sure it's spot on. We also installed a grid of 30 drill bushings in the table to use as absolute known alignment positions for our vacuum fixtures. This allows us to use bullet nosed fixreture dowels, two per fixture that mate with bushings in the underside of the fixtures. Basically, the first layer of any CAD drawing becomes the table and it's drill bushing locations, then the fixture, then the part. Works great, and the XY 00 is always the same...that corner of the vacuum table...no matter where the fixture is.

I would love to see some pictures of your setup and how if functions. I need to install something like that into my new vacuum plenum strips. Maybe a couple screen captures of your CAD setup with the bushing locations as well?

Thanks!