Is it possible to call variables in the post from a tool other than the active tool?
I am setting up a post for our laser now and the only way i can figure to make this work easily is to use a different tool for each different material. I have a tool set for each different thickness material with custom parameters like power, frequency, duty cycle, feed rate, gas type, nozzle size, pierce dwell, etc. I really need a material table separate from the tool table, but just using the tool table works… until i need to etch something before i make a cut.
The etch tool always uses the same parameters regardless of material. Problem here is, my post initializes the machine with the parameters from the first tool called. When this tool is the etching tool, all the parameters to cut the material later are wrong and cannot be reset.
I see in the documentation that there is a variable “tool” which is the current tool number and “nextTool” which is the next tool to be called. Is it possible to call a variable from the next tool? something like post.NonModalNumber(“M134 P”, tool21.power, “0000”)
Thanks,
David
Unfortunately not. It should be possible to get the standard values such as feed rate, pierce delay etc but not custom values defined in the post.
Ok. Perhaps something to consider adding in the future, though its probably not worth the development. What i am doing is likely a very limited application of SheetCAM.
As a work-around, i created a post variable that tells the post if the operation is an etch or cut. Just requires an additional step in the operations sequence, but no big deal at all.
Can you use the plate marker tool for the scriber? You can detect the tool is a scriber like this:
if toolClass == "ScriberTool" then
end
You can also add parameters in the same way as for other tools.
I dont believe i can because the scriber is another tool. I am using the tools as a material database instead of as actual tools. That is why i was saying it would be beneficial to have a separate material database with customizable parameters just like the tool database.
The way our machine (Mitsubushi ML3015ex plus) works is there are numerous cutting conditions. There is a separate file for each material thickness and gas and nozzle configuration. These files have 11 separate cutting conditions detailing power, frequency, feed rate, etc. One of the 11 is the pierce condition and another is the etch condition. the other 9 are cutting conditions.
There are a few options.
Instead if using the normal functions to write to the post file (post.Text, post.ModalNumber etc) you could stuff everything in a text string. Append each line to the string. When you hit the tool with the settings, stick that data at the start of the string. It’s a bit ugly and you lose the useful functionality of ModalNumber etc.
Another option is to use a two-pass technique. Keep most of your post as-is but don’t output the tool information in OnToolChange. Now in OnFileClosed() read in the contents of the file, add the settings and write it out again. Take a look at the Biesse Rover XNC post for an example of that trick.
I am not fully comprehending what is going on in that post right now. It seems to be a little over my head for the time being. I do not see what exactly is being replaced and what it is being replaced with. Perhaps i can just generate some gcode and figure it out, but that will have to wait for another day with more free time.
The set post variables method i came up with seems to be working well for now. Hopefully i can revisit this soon though.
The biesse Rover XNC controller uses a bastardized version of g-code where some values at the start of the file need to point to the byte offsets of parts of the g-code. These values can only be known once the file has been created. The Italians are experts at mangling g-code and this horrible mess is a prime example.
In that post take a look at OnFileClosed(). It reads the g-code file into a string. It then plays around with that string to replace dummy values with the actual values then writes it back out.
In your case you could write the post to only output the stuff after the tool configuration data. Then in OnFileclosed you could read the g-code file in, add your settings to the start of the string and write it back out. Lua is a general purpose programming language so at this point you are just doing normal string manipulation.
Ahhh, i see now. That makes a little more sense. I was trying to picture what was being written without actually writing a code and it did appear to be a jumbled mess. Ill take a closer look later this week. Thank you Les
Another Mits user here, stumbled across this and wanted to followup. Did y’all get this all figured out?
Our controller is different (looks like you’re the next gen, we’re just LC20), but we can call various material files and then various parameter lines from G-code directly. We’re actually running generic tools (I have a mits 0 diameter and a mits .001 diameter, and that’s it).
I forget the exact syntax to pull a material file (we just usually pre-game that manually), but the variable (#501 i think) will call a parameter line. I.e. #501=102 calls up line 2 (usually our etch line), or #501=107 is our balanced cut condition. We use this to flip between lines for fast cut, slow cut, peck cut (occasionally), and etch for a given feature. I haven’t tried doing it mid-cut with code (but I have called manually, so the controller might support it). Currently our post calls it right before the pierce line.
Coming from BobCAD the power and documentation for SheetCAM’s post processors makes my head spin!
As @Les_Newell described a couple of solutions 5 years ago which would still be valid today, I don’t see him mention a post processor function DefineCustomToolParam(), so odds are it’s been added since 2019. This function allows the pp to add parameters to tool definitions by tool class, ‘LaserTool’ for example, or ‘PlasmaTool’.
The pp has read access to those custom param values when the tool is the active operation tool. An alternative solution may be that you add the 11 additional params to your tool defs and thus have what you need when you need it. Using OnToolChange(), read the custom params and write the string as gcode line, saving the line number for use prior to the pierce.
never mind my prior post, after re-read of prior solutions, I see the use of DefineCustomToolParam() is implied and in use already.
@Bookmann Sorry, but I don’t work for that company any longer. I left about 9 months ago. I worked with Les a lot to get a functioning post processor with everything I wanted to do. He was extremely tolerant of my requests lol. I ended up writing custom posts for all of our machines, we had 2 plasmas, a waterjet, the mits laser, and a router table just because i like to get very creative make the machine do all the work for me instead of unnecessary additional labor haha. I’m sure Les can attest to that with some of my unusual requests haha. I honestly cant remember what all i did, but i know a couple of my custom posts accidentally made it into Les’s official release of sheetcam. If they’re still there, they would be a number followed by a machine description something like “004-Waterjet no ITC” was one i think or “010-Laser with comp control” was another maybe. If they’re still there you’re welcome to use them as examples or modify as you see fit. If i think about it later and i can find my old flash drives, i’ll PM you what i may still have.
I do remember i had quite an intense tool table in sheetcam. Basically i had a tool for every material, thickness, and gas combination. It worked really well and made it pretty dummy proof for the operator. As long as he actually read the setup report sheet and loaded the correct material, it always cut.
Hey, I appreciate automation - I’m just not used to having all these options, haha! I haven’t even started trying to grok code snippets, cutting rules, or the advanced bits of posts or the tool table…
Thanks for the heads up about those posts, I’ll poke around in/with them and see what I can figure out. Les & crew will probably have some more crazy questions to keep them on their toes.
Best wishes moving forward.
