[shorton]

That IS what I meant in both cases, thanks very much.

After I thought about it seems it would be very difficult to simulate the macros I'm fiddling with anyway without having some means to send signals from the PP driver. And that would be a PITA even if I could do it. So I'll stick to attached to the machine for testing. I can remote to the machine from my desktop when I don't want to sit in the shop (machine on estop of course)

Cheers

[shorton]

Excuse the approaching off topic question.... When programming these macros, I've watched you save variables using the set/getOEMDRO functions so they are non-volatile and save the value across starting and stopping the software. If I want to save one using the setoemdro() function, do I have to have a screen DRO to match it? Or can I use it regardless of the existence of a corresponding screen DRO? If I can, I figured I'd see which ones are used across all the macros in use, and then pick a number maybe 10 more than the last "custom" number used, that does not conflict with any published DRO number of course.

[ger21]

You can send and recieve signls to/from the parallel port driver by checking the "emulate" box in ports and pins and assigning a hotkey to them.

And yes, you need to have the DRO in the screen for it to work. (At least I'm pretty sure you do.)

[shorton]

re PP pins, Cool, thanks.

I did find the setOEMDRO "sticks" without a corresponding screen DRO.

For my
setOEMDRO(1820,1239)
After closing Mach 3 and looking at the XML, it lives at:
OEMDRO2_565

Odd where it puts it in the XML though. I'm sure there's a starting point/formula to get from 1820 to 2-565. So unless 1820 is used by the system (?), I'm OK
Looked like the last one you used was 1814.

[ger21]

I'd stay out of the .xml.

1820 is what you need.

[shorton]

Yep. No plans to mess with it. Just wanted to see if the thing got stored. Roger 1820, thanks

[nc42]

This looks pretty cool. I'm just putting together a machine and haven't used Mach 3 but planning on it. I have one question about the auto tool measure. Is it able to go to touch plate for measuring new tools even if you set the x,y zeros to some where other than the origin or do you need to reset the location of the touch plate. I'm guessing it has this feature but just wanted to check.

[shorton]

I'm new at using Gerry's screenset but think I can answer. With this excellent addon you set the X-Y location for the reference plate location. I'm modifying mine a little but for mine and stock, it does not matter where you start from, when it's time to take the reference plate measurement, it goes there. YOu only ever set it's location once.

[ger21]

Sorry for the late reply.
The fixed plate location is specified in machine coordinates. You'll need home switches to provide repeatable machine coordinates.
Let me know if you have any other questions.

[shorton]

Gerry, et al. :

I know I've expressed it before but I have to say it again. I'm tickled pink with your screen set and the ability to tweak the macros I want to fit my work. The programming language was very generic and although technically new tome, very straightforward. Gcode as well, pretty straightforward for what's in the macros I use anyway. Armed with all this new power I was able to tweak my whole setup to do just what I like.

For my CNC router we are usually changing materials out quite a bit. Sheet goods from 3/4 pine to 1/8" PVC. After giving some consideration of the pros and cons, I believe I am going to shif to building my CAM files with the table as Work Z0. I use CamBam for my CAM, and use its profiles fully. The profiles are tool, material, and material thickness specific. For example 1/8" Bit, Wood, 3/4" thick. In those profiles I preconfigure things that don't change, like S&F, target depth, and material surface location. In the profile I set the material surface a little high so worst case, I cut a little air before the bit makes it to the material. Best case or as needed for more precise top-down needs, I fine tune to the gcode file to the exact material thickness that's on the table. With this method, I only have to probe the table one time to determine Work Z zero and the distance between the table and the reference plate. Once probed, these are always constant unless I change the table (e.g. reskim it), or I choose to set Z0 to a material's surface.

CamBam creates an initial tool change in it's gcode. I have a postprocessor executable that takes that output and filters out that first tool change automatically. I don't have to touch it or do anything special other than configure the processor once.

My machine has a isolated spindle and requires a clip when probing.

My modified 2010 Screenset, related options (for my setup) are:
Material Offset (check or not and enter thickness of work material to run gcode that expects work surface at Z0). For table referenced work, uncheck. Haven't completely tested this, but so far appears to work correctly.
Manual Spindle control checked - when checked you get the prompts to attach and detach clip
Ignore M6 calls unchecked. If you check it, it pretty much disables all the auto-zero stuff in all macros

My new workflow is as follows:

1. Power the machine on,

2. Reference all home (RAH) macro (M884). That's business a usual but now I have edited this macro to include a tool probe to my reference plate. So I get a reference on X, Y, Zref, and Ztool. At this point the machine does not know the reference plate to work surface delta, but the last one is still stored in a DRO 1820, so I read that in as a possible start point. If the tool did not change since last time I probed the table, technically, that value is still good. Subject to variations in my limit switch trigger at RAH. But the primary function in this macro is to get the machine coord for the tool touching the reference plate.
When probing the reference plate, I know about where it is, so the spindle is moved to the probe point, moves down faster than stock (distance determined by using the machine's Z soft limit) to just above the fixed reference plate. Once close to the plate, then prompts to attach probe. It probes as normal. Then it retracts just a little and prompts to detach probe. My RAH macro parks after referencing the 4 points. By having it closer to the reference location before prompting for probe clip attachment and removal, it doesn't drag the wires around the table, over a part, etc.

3. Jog to an open area on the table (or material if I wish)

4. Run My Initial AutoZero macro (M881). My version is also different than the stock version. Mine only probes for the table/work surface instead of both the table/work and the reference every time. I already know the reference plate height from the initial RAH macro. On startup it prompts to connect the probe clip and position the touchplate. After probing the touchplate, the delta from the reference plate and table/work is recorded in DRO 1820. This macro probes slowly as normal, from it' start point because it does not know where the surface is. When complete it acts similar to the RAH macro, retracts just a little prompting to remove clip. Then it parks.

5. Jog to the work, set X and Z zero.

6. Cycle start. Cuts MOPS with 1st tool

7. When/if my setup encounters a tool change in the Gcode it kicks off the M6Start and M6End macros. M6Start retracts to the tool change position and prompts the user to change tools, click OK when done. Change tools, click OK, it kicks off the M6End Macro. There was some concern about this because I have the M6Start "feed" a cycle start to M6End. For what it's worth I've done it 50+ times now and it has never worked incorrectly. So I *think* it is OK. But a reader copies this setup, do at your own risk of course. M6 End now moves the tool to the reference plate, and calculates a new delta between the new tool and the table/work. Adjusts the Work coordinate system accordingly. The work/table haven't moved and do not need to be reprobed. After the tool (re)probe, which also works like the RAH macro, the user removes the clip, clicks OK, and the machine cuts the next MOPs with this tool.

8. End of job, CamBam gcode footer kicks off a M883 to park my system.

Now, since I'm referencing the table as work Z0, I can change material and never have to re-reference the Z0 for the work. If the tool changes in a gcode file, the system auto-calibrates to the reference plate, still no need to probe the work.

Once I RAH, then set initial zero, everything else is automatic, requiring no subsequent probe. Even if I change material.

The only time I have to do both steps (Ref All Home with ref probe, Auto Zero with table/work probe) is when I power up, or I've stalled the machine, etc.

For times I want to reference the top of the material as Z0, then I have to probe it with auto-zero once per material change.


Best part:

Next Job (if I didn't change tools in between), I change material. I load the gcode file, I press cycle start. Work Zero is already known. No probing needed.

Next Job (if I did a tool change between jobs), run auto zero, I get one quick automatic probe to ref plate, cycle start, done.



Beautiful.

Just have to decide what I'll do with the normal reference button.

Thanks Gerry!



Gerry. Since this is your thing that I've modified, I won't post the associated 4 macro files unless it's OK with you? Happy to share with you off-line if you'd like to check them out. I'll try to get a video of my start to finish modified process.

[ger21]

You're free to post the macros anywhere you'd like. They started with macros posted by others, so feel free to share them with the community.
Even though I spent about 3 weeks getting the macros to do what I wanted, the $20 fee is to cover the 3-4 months I spent on the layout and graphics work.

Material Offset (check or not and enter thickness of work material to run gcode that expects work surface at Z0). For table referenced work, uncheck. Haven't completely tested this, but so far appears to work correctly.

Not sure if I follow you, but I'll add a little more info.
Material Offset is actually a Z zero offset, offsetting Z zero by the value entered. You can use it to get the same effect as zeroing to the table.

What I do, when I'm cutting 3/4" parts, is program them as if they are always exactly 3/4" thick, even if they are a little thicker or thinner. If I'm cutting all the way through, I might program my depth of cut to -.745, so I don't quite cut into the spoilboard.
I set my Material Offset to .75, and zero to the spoilboard or table. This sets Z zero .75" above the table, so my "through" cuts are always .005" above my table.

The only time this doesn't work is if you're V Carving, or need pockets of a precise depth. In that case you must know the exact thickness of the material, and program accordingly.

[shorton]

You're free to post the macros anywhere you'd like. They started with macros posted by others, so feel free to share them with the community.
Even though I spent about 3 weeks getting the macros to do what I wanted, the $20 fee is to cover the 3-4 months I spent on the layout and graphics work.

Thanks. I didn't want to without asking first. As for the $20, you don't charge enough. Took Mach3 from something I wasn't really crazy about to a very comfortable interface.

What I do, when I'm cutting 3/4" parts, is program them as if they are always exactly 3/4" thick, even if they are a little thicker or thinner. If I'm cutting all the way through, I might program my depth of cut to -.745, so I don't quite cut into the spoilboard.
I set my Material Offset to .75, and zero to the spoilboard or table. This sets Z zero .75" above the table, so my "through" cuts are always .005" above my table.

Excellent, that is exactly what I had in mind to do when using it.

The only time this doesn't work is if you're V Carving, or need pockets of a precise depth. In that case you must know the exact thickness of the material, and program accordingly.

Yes, I considered this when I did my pros and cons comparison. For a precise pocket depth one will need to get the offset about perfect, or zero to the surface. I haven't gotten Vcarving, yet.

I'm going to test a little more with my offsets. Make sure I didn't miss anything in my macro, then I'll post. I admit there was some serious head scratching and sketching being done as I figured it out and worked with the dual coordinate system arithmetic LOL.

[ger21]

I admit there was some serious head scratching and sketching being done as I figured it out and worked with the dual coordinate system arithmetic LOL.

Yes, I drew a LOT of sketches when I first did the macros.

[shorton]

OK, here is my modified 2010 AutoZero system. It's missing metric handling, I don't use metric. It will be trivial to add to the macro's if someone needs it. My macros are heavily commented so that when I look at them the next time (or someone else does), I can hopefully figure out what I'm doing .. I used the naming convention when referring to the Z axis of ZW[varname] for something that is in work coordinates, ZM[varname] for something in machine coordinates, and ZD[varname] for something that is just a distance, not tied to a coordinate system.

Again, in summary mine works like this:

1. M884 - reference All Home. This is tied to Gerry's "Reference All Home" button. Mine references X-Y-Z, but also references the machine coord (ZM) of the current tool as part of reference all home.

2. M889 - reference Z work (ZW). This is tied to the single chevron button (formerly simple auto zero). My macro probes for ZW zero, which for me is the table, but can be the work surface as you prefer. Calculates and stores the delta from ZW0 to the reference plate Z. This calculated value is used with subsequent tool changes.

3. M6Start/End; Tool Change. These are tied to M6 commands encountered in the gcode. They cause a move to the tool change position, after tool change an automatic touch off to the reference plate, and an ZW autoadjustment so the new tool is aligned with the current ZW coordinate system. No ZWork touchoff required.

4. (NEW) M889 Toggle Material Offset: My setup freed a button on the original screenset, the "Double Chevron" (formerly the Initial auto-zero button). I programmed this button to be a material offset toggle button. I think the material offset toggle kinda fits the graphic of the double chevron (either something stacked or not). Anyway it works like this: If you used the material offset when the initial Work Zero was run (#2 above), then that was recorded at the time. Clicking the double chevron sees that offset, prompts if you would like to remove it. Answer yes and it takes it away. Sets ZW0 back to no material offset location. If you had not used any material offset, but now want some, clicking this button senses no offset ans asks if you want it. Answer yes and it adjust ZW0 to include the material offset as entered in Gerry's tool change DRO. So this is a one-button, no probing required way to turn material Z-offsets on or off as needed.

I've tested them pretty well. I'm subject to find some unanticipated anomaly, but they seem to work correctly for all normal cases. All of them take into account the need for attaching probe clips if you have a insulated spindle, stop the spindle at appropriate heights close to the work to clip/un-clip. Just click "Manual spindle control" to enable that.

These fit my workflow well, maybe they will help someone else, posting here if you want to try them. Should someone try them and find an issue, let me know I'll try to fix.

Thanks again to Gerry for the outstanding framework that made this possible for me to do, with only a little programming which I'm OK at. And for the little bit of hand holding I needed to get started.

Cheers


P.S. Gerry: regarding that "push" of the Cycle Start we discussed previously. I found the thing that caused it to not work correctly. It only happens if I try to run the M6Start macro in the debugger. In that case cycle start isn't branching to M6End, so it started the spindle as if I pressed cycle start from an idle machine. I'm feeling pretty good about the feeding of cycle start by M6Start now. Hasn't messed up when triggered correctly (via gcode M6 call).

Edit: Revised files. 2 had ending debug messages, removed now. sorry bout that....

[shorton]

Updated Video of my macros working (apologies for lack of close-up focus, but you can "see" what's going on):

https://youtu.be/4cqSZBpCKW4

[matth]

Hi Gerry, can you recommend the best way to actuate your custom buttons from an external physical button?

I use a Pokeys56u for my control panel, most things can be actuated with the Mach3 plugin or a key press I.e. Carl+p for Park. But I'd like to assign buttons to simple zero, TC, ref all home etc.

Is there an easy way to do this? Is there keystrokes in the background for these buttons!

Cheers,

Matt.

[cd_edwards]

Hi Gerry, can you recommend the best way to actuate your custom buttons from an external physical button?

I use a Pokeys56u for my control panel, most things can be actuated with the Mach3 plugin or a key press I.e. Carl+p for Park. But I'd like to assign buttons to simple zero, TC, ref all home etc.

Is there an easy way to do this? Is there keystrokes in the background for these buttons!

Cheers,

Matt.

I just recently added a button on my spindle head todo the initial auto tool zero function. It took a lot of tinkering to get it working properly. My understanding is that poppa bear's mad4mach3 makes it easier as well as allows more buttons. I only required one. My understanding is that you can only have 1 trigger macro active. So.

System Hot Keys. Not sure why this is, but without it, you will not get it working.
OEM Code 10 set to 301

Now in Setup -> Input Signals -> OEM Trig #10 set to a port/pin and correct Active Low This is your switch.

Create a M1000 in your config directory. IE C:\MACH3\macros\Smooth-VFD

'M1000.m1s (in the init line)
SetTriggerMacro( 1001 )


Create a M1001 in the same directory.

'M1001 This calls M881 which is the initial tool set

If isActive (OEMtrig10) Then
Code "M881"
End If

And finally add M1000 to your Initilization string in Config->General Setup

And then there is the brain you need to make.
OEM Trig 10 -> Invert Flip Signal -> Execute Button Script

[ger21]

Matt.

The easiest way is to add hotkeys to the buttons. You can do it in a screen designer, either Screen 4 or Machscreen.

Colton,
I recall that there's a slightly easier method than you used that doesn't require the use of a Brain. But you are correct, in that you can only use it to call a single macro.

[matth]

Matt.

The easiest way is to add hotkeys to the buttons. You can do it in a screen designer, either Screen 4 or Machscreen.

Colton,
I recall that there's a slightly easier method than you used that doesn't require the use of a Brain. But you are correct, in that you can only use it to call a single macro.

Thanks Gerry, I will give that a try and come back and ask a load of questions when I get it wrong!

P.S. I use your screenset every day and it really has changed the way I view Mach3. It is such a usability improvement. Thanks for all your hard work on it.

[matth]

Added the hotkeys as suggested, all worked a treat. Thanks Gerry.