|
I mean, I can print polysulfone, which is designed to be autoclaved. Depends on budget and quantity
|
#
?
Jun 5, 2021 20:22
|
|
|
|
| # ? Apr 26, 2024 00:58 |
|
|
Looks like I can buy some of that in filament form for $69. LoL! 3/5 stars on fake Amazon reviews. I have an enclosure for printing ABS. What's the word?
|
|
#
?
Jun 6, 2021 05:08
|
|
|
Dominoes posted:Looks like I can buy some of that in filament form for $69. LoL! 3/5 stars on fake Amazon reviews. I have an enclosure for printing ABS. What's the word? Unless you have a printer with a heated chamber that can extrude at 380c and have a bed temp of 140c, the word is lol. I have experimented with high temp filaments like this and even on a heavily modified printer that can hit the extrusion and bed temps they are pretty much unprintable without the heated chamber.
|
|
#
?
Jun 6, 2021 15:56
|
|
|
Dominoes posted:Looks like I can buy some of that in filament form for $69. LoL! 3/5 stars on fake Amazon reviews. I have an enclosure for printing ABS. What's the word? uh, you're not going to be able to print that. It was more "if milling aluminum fails, let's work something out for me printing it"
|
|
#
?
Jun 6, 2021 23:51
|
|
|
It arrived! Changed plans a bit so Im going to have to prep a different spot for it than I first thought but its here!
|
|
#
?
Jun 8, 2021 16:50
|
|
|
Okay, I don't mean this the way it'll probably read, but: What the gently caress?
|
|
#
?
Jun 8, 2021 19:07
|
|
|
It's a CNC router kit! Send progress pics OP!
|
|
#
?
Jun 8, 2021 19:28
|
|
|
NewFatMike posted:It's a CNC router kit! Send progress pics OP! Oh! https://www.onefinitycnc.com/product-page/build-your-own-onefinity $2,100 + shipping for all the bells and whistles they offer for a 32 1/8"(X) x 33 1/8"(Y) x 5 1/4"(Z) work area kit isn't bad. Having the controller built-in at that price and not having to kludge one together is pretty neat, too. Wish this was available to add to it: https://www.onefinitycnc.com/product-page/woodworker-qcw-frame-secure-from-above-version but I guess waiting until it's available and then budget-checking wouldn't be a hard sell. EDIT: The controller itself is $500 directly from Buildbotics. https://buildbotics.com/product/113/buildbotics-cnc-controller
|
|
#
?
Jun 8, 2021 19:51
|
|
|
Will update once I have it up and running. Seems very solid so far.
|
|
#
?
Jun 8, 2021 23:01
|
|
|
Re post-processing: When I click "Post-process" in SolidWorks (using the "M3AXIS-TUTORIAL" post-processor), and save as a .nc file, it looks like the files I've been making with the script. It can be opened by Candle, showing what looks like a correct graphical representation. Is there a reason for a separate GRBL post processor? Maybe there are special dialects like for 3d printers that are different (I don't know how you'd command a 3d printer using the code I learned), but CNC has common standards? Ie, SW is generating the standard G01 for straight moves, G02 and G03 for arcs, coordinates for these using (X, Y, Z, I, J), F for feed rate, S for spindle speed, M03 to turn on in a certain direction etc. It looks like SW is also generating commands for coolant and changing tools. And, the S and F settings are 10x higher than I've been using. (And probably not something the 3018 pro can handle; need to go back to the mill config) NewFatMike posted:I haven't tried any metal in my 3018, but if you find a GRBL post processor, let me know, because that'll save me a lot of guesswork in making one insta posted:uh, you're not going to be able to print that. It was more "if milling aluminum fails, let's work something out for me printing it" Dominoes fucked around with this message at 03:40 on Jun 9, 2021 |
|
#
?
Jun 9, 2021 02:49
|
|
|
If M3AXIS Tutorial works, that whips. I'll have to see how it handles canned cycles because I don't think any of those are supported by GRBL. Definitely check it out, and I'd love to hear a trip report! E: Candle works, as does universal GCode sender IIRC. It's just a motion controller software.
|
|
#
?
Jun 9, 2021 05:12
|
|
|
Dominoes posted:Re post-processing: When I click "Post-process" in SolidWorks (using the "M3AXIS-TUTORIAL" post-processor), and save as a .nc file, it looks like the files I've been making with the script. It can be opened by Candle, showing what looks like a correct graphical representation. Is there a reason for a separate GRBL post processor? You have fundamentally misunderstood my post about what a post-processor is. Solidworks creates its own toolpaths in machine agnostic format. This is its CAM process. It then post-processes its intermediate files into e.g. GRBL gcode. So there isn't an additional piece of software after it comes out of solidworks. Just because the .nc appears to be gcode "like the files" you've been making, doesn't mean that every machine-agnostic instruction will be translated properly by the "M3AXIS-TUTORIAL" post-processor into stuff that GRBL understands. If this happens, then the best possible thing that can happen is nothing. A much more likely thing to happen is a powered milling move into something you don't want milled. A surprisingly common thing is a full-speed move back to a home position while at maximum depth with the spindle spinning. If you're lucky, you stall out the machine. Not lucky and you break a tool. Unlucky and you break the machine. So yes. It is moderately to very important to use the correct postprocessor for the specific gcode flavor your machine speaks. edit: How about an example. Say you want to drill a hole. You tell SolidWorks that you've got a 1/8" drill bit, and please drill a hole at some place. There's a distinct possibility that the "M3AXIS-TUTORIAL" processor will output a G81 Canned Drill Cycle (or G83 deep drill with chip breaking). GRBL doesn't know what a G81 means, so it (hopefully) throws an error. If it doesn't throw an error, then what does it do? Only GRBL devs know, but it almost certainly won't drill a hole. At worst, it'll move to the XYZ location of the G81, which is the bottom of the hole, thereby driving your drill bit sideways at rapids speed into your work, breaking it and making a wonderful scratch. I'll let someone else address the speeds and feeds being higher than you're using for reasons you don't understand. babyeatingpsychopath fucked around with this message at 08:25 on Jun 9, 2021 |
|
#
?
Jun 9, 2021 08:10
|
|
|
Your CAM software controls what values output for things like safe retraction points/etc. (otherwise there would be no point in making sure you define those values in your toolpath dialogs in the CAM software). As an aside, I always make sure the NC tab on any Toolpath in Solidworks CAM/CAMworks is set to "Top of Stock" for the reference for all retraction plane data (there are options for "Top of Feature" and "Last Cut" depths that might be useful in very narrow application ranges but will always result in a crash if your features are ever below the top of your stock definition). The M3AxisTutorial post processor just outputs your basic (and I do mean basic) G/M-codes with X/Y/Z and S/F/etc. values where appropriate and doesn't do any special flavor stuff like specifying lookahead values (for machines that support it) or any definition values (for the machines that don't store that information in firmware by default) for things like acceleration/jerk/etc. It's also pretty much based on the FANUC standard G & M-code list, which is the same as about 99% of all milling machines and lathes out there built after February 1980. You know, RS-274-D (the standard code table used by every manufacturer of CNC controllers on the planet, copied and renamed to ISO or DIN or whatever, but the actual codes are the same). Things like how many significant digits to use for spindle speeds and feedrates are things that are machine-dependent and you can compensate for a post-processor outputting "wrong" values by editing your post processor in most cases (or you can just subtract however many significant digits from the spindle speed and feedrate yourself to get the values you actually want in code (just move your decimal point accordingly). The only time this differs is if you get a machine that doesn't have a particular feature-set enabled because the software front end wasn't developed to take advantage of it for the operator, or the machine lacks the hardware a specific code would reference so calling it up will just cause the machine to stop and wait for input/error out of the program and require re-homing to a safe position. Like, not having a tool library definition in the machine because there is no tool carousel or tool holder setup with probing tools to take advantage of--a poorly configured machine setup will misread cutter comp code such that the value after the letter D will be interpreted as the actual diameter of the tool rather than the tool number reference. This can be compensated for in your post-processor definitions, assuming you have access to editing software for the post processor--something CAMWorks won't share with the end user because creating and editing post-processors is their bread-and-butter unless you want to try your hand at configuring a post from scratch with their post processor generator software--but it's the kind of thing to watch out for when using generic post-processors. If you want to try your hand at making your own machine-specific post-processor you can download the "Universal Post Generator" here: https://camworks.com/universal-post-generator/ But good luck doing that because CAMWorks VAR are basically "You can do that at your own risk, we aren't supporting the end user who chooses to play with that" (same policy they take about modifying the Setup Sheets to do what you might want to do). Some Pinko Commie fucked around with this message at 12:44 on Jun 9, 2021 |
|
#
?
Jun 9, 2021 11:29
|
|
|
FWIW, the UPG and EC Editor are what we use on the VAR side. I'm not sure if CAMworks train folks on it (I sure haven't been offered any training from them). I shouldn't have responded to the post right at bedtime, I thought it was in a much better place. Test new code, post processors, etc. with stock and tools you won't mind losing 
|
|
#
?
Jun 9, 2021 13:45
|
|
|
NewFatMike posted:FWIW, the UPG and EC Editor are what we use on the VAR side. I'm not sure if CAMworks train folks on it (I sure haven't been offered any training from them). Of course. I'm just aggravated because we no longer have support for the post-processors (purchased while I was out of work on a medical thing and the support period expired during that time) and I'd like to make some changes to them, but they refuse to share the source files with me so I'm not starting from scratch. I got the setup sheets to work halfway like I want them to, but it took some deep diving into the XML output in Solidworks files (and some time invested into teaching myself how to format XML and XMLT files) to figure out the different variable names for things I want to show on the setup sheet and then format everything to display/print properly.
|
|
#
?
Jun 9, 2021 15:03
|
|
|
NewFatMike posted:If M3AXIS Tutorial works, that whips. I'll have to see how it handles canned cycles because I don't think any of those are supported by GRBL. babyeatingpsychopath posted:You have fundamentally misunderstood my post about what a post-processor is. biracial bear for uncut posted:Your CAM software controls what values output for things like safe retraction points/etc. (otherwise there would be no point in making sure you define those values in your toolpath dialogs in the CAM software). As an aside, I always make sure the NC tab on any Toolpath in Solidworks CAM/CAMworks is set to "Top of Stock" for the reference for all retraction plane data (there are options for "Top of Feature" and "Last Cut" depths that might be useful in very narrow application ranges but will always result in a crash if your features are ever below the top of your stock definition). I'm hoping I don't run into the adverse reactions you describe! If it looks like the software or machine ignore bogus commands, I'll make a decision of removing them, or letting them be. NewFatMike posted:Test new code, post processors, etc. with stock and tools you won't mind losing Thanks so much dudes! I'll keep you posted.
|
|
#
?
Jun 10, 2021 01:02
|
|
|
Where I work there are two FANUC machines with nominally the same controller hardware, but with two key differences regarding spindle speed and feedrates. The one machine requires a code output with two zeroes beyond your intended whole number RPM target. So 17,000RPM would be output as "S1700000". 17,500 would be S1750000, etc. The other machine takes whatever value is supplied in the code and multiplies is by 1,000. So 17,000RPM would just be "S17". 17,500RPM would be "S17.5", etc. Feed rates in inches per minute work the same way for the first machine. A feedrate of 200 inches-per-minute would be "F20000", 260 inches per minute would be "F25000", etc. On the second machine, 200 inches per minute is "F200.", 250 inches per minute is "F250.", etc. Note the decimal points when present, because they are important. For your examples, T01 and M06 tell the machine to check what tool is currently present and change tools if the current tool doesn't match the callout. So if "Tool #1" isn't defined, or that machine isn't set up to use a tool changer, the machine will ignore both codes. M08 means "turn on flood coolant", so if your machine isn't set up for that it will do nothing. A bad machine firmware setup that has the option for coolant enabled, but lacks the hardware, will throw out errors and halt the program.
|
|
#
?
Jun 10, 2021 01:48
|
|
|
That's hilarious re the settings! (Though, I speculate you harbored no feelings of amusement when discovering this). I hope this equipment will ignore the T06, M06, and M08 commands rather than do something undefined. We'll see! Perhaps the designers of this machine decided that M06 means "Ops test maximum spindle and feed speeds across the entire range of motion, bottom-first" Dominoes fucked around with this message at 02:05 on Jun 10, 2021 |
|
#
?
Jun 10, 2021 02:02
|
|
|
Dominoes posted:That's hilarious re the settings! (Though, I speculate you harbored no feelings of amusement when discovering this). I hope this equipment will ignore the T06, M06, and M08 commands rather than do something undefined. We'll see! I have a GRBL 3018. I keep M06/M08 in as a final "sanity check" that everything is going fine, and maybe to turn on the vacuum. GRBL spits out an "unknown command" warning which candle catches and lets you bypass. Since GRBL doesn't understand whatever M-code "pause and wait for a continue" is, M06 or Txx works well for that. I also have a tool library in Fusion with the actual tools I own; the fusion # is written on the box/location the tool is in. When I see the "unkown command T201 ; quarter-inch 3-flute endmill" I look over and verify that the only empty slot in the tool holder rack is #201.
|
|
#
?
Jun 10, 2021 07:27
|
|
|
babyeatingpsychopath posted:I have a GRBL 3018. I keep M06/M08 in as a final "sanity check" that everything is going fine, and maybe to turn on the vacuum. GRBL spits out an "unknown command" warning which candle catches and lets you bypass. Since GRBL doesn't understand whatever M-code "pause and wait for a continue" is, M06 or Txx works well for that. That would be M01 (literally coded as "optional stop") where the machine will stop and wait for the operator to hit cycle start again (unless some lunatic disables that option at the controller).
|
|
#
?
Jun 10, 2021 10:36
|
|
|
Looks a bit more like an actual machine now   Went together very easy. A handful of bolts and screws basically. They recommend a specific order to ensure alignment. Seems to have worked. Probably not its permanent home, but I wanted to get it put together to make sure everything works properly. Got a little cable management to do, but nothing unexpected. Turned it on, booted up, homed it no problem. Now I'm crippled with choice paralysis as I start trying to pick which of the projects I have in mind to start on. Going to start with a few basic test cuts but I should be able to do something this weekend with it.
|
|
#
?
Jun 10, 2021 20:49
|
|
|
Tested the default-ish SolidWorks post-processing with Candle and the 3018 pro. Works fine after I change the spindle speed line in the resulting file to S1000 instead of S10000; I get an error I can ignore in Candle about the unsupported commands.
|
|
#
?
Jun 13, 2021 02:58
|
|
|
Is that the M3AXIS TUTORIAL one?
|
|
#
?
Jun 13, 2021 05:32
|
|
|
Dominoes posted:Tested the default-ish SolidWorks post-processing with Candle and the 3018 pro. Works fine after I change the spindle speed line in the resulting file to S1000 instead of S10000; I get an error I can ignore in Candle about the unsupported commands. If you ever try to calculate the correct feed and speed for that 3018, be mindful that you have to run the spindle at 100% all the time, because if you PWM it below about 90% it loses all of its torque and stalls. Do a lot of air cuts to make sure the machine is doing the things you expect it to.
|
|
#
?
Jun 13, 2021 06:50
|
|
|
So I'm interested in getting into CNC machining. Pobably staring with a normal desk sized 3 axis, but possibly with an eye toward adding extra axes. So my question is: how do you typically go about expanding the use of a machine to 4th or 5th axis. Do you install them into the gantry? Or add them to the table like this?
|
|
#
?
Jun 13, 2021 08:35
|
|
|
NewFatMike posted:Is that the M3AXIS TUTORIAL one? edit: Solved - "Curve" is the right feature type. babyeatingpsychopath posted:If you ever try to calculate the correct feed and speed for that 3018, be mindful that you have to run the spindle at 100% all the time, because if you PWM it below about 90% it loses all of its torque and stalls. Dominoes fucked around with this message at 15:11 on Jun 13, 2021 |
|
#
?
Jun 13, 2021 14:47
|
|
|
The Atomic Man-Boy posted:So I'm interested in getting into CNC machining. Pobably staring with a normal desk sized 3 axis, but possibly with an eye toward adding extra axes. So my question is: how do you typically go about expanding the use of a machine to 4th or 5th axis. Do you install them into the gantry? Or add them to the table like this? Machine axes configuration beyond the normal 3 axis milling setup depends on what you'll be machining and the intended uses of your machine. Things get much more complicated when you add 4th and 5 axes tool paths. Most people don't add a 4th or 5th axis ever. You're getting way ahead of yourself, spend some time making parts first. This question would be like saying "I'm thinking about buying my first car so I can learn to change oil, how do typically install fuel injection on a carbureted car?"
|
|
#
?
Jun 13, 2021 15:11
|
|
|
Always make sure your NC output is set correctly on the NC tab on the Toolpath options. I always go with "Cutter Comp Off" and whatever the wording is for "Output Code with Toolpath Centering" or whatever. If your cuts are coming out big then the cutter comp codes are on but your machine has incorrect values for tool diameters. And you may want to read this for a better understanding of the different operation types. https://www.goengineer.com/blog/camworks-milling-features-and-allowable-operations Some Pinko Commie fucked around with this message at 15:26 on Jun 13, 2021 |
|
#
?
Jun 13, 2021 15:21
|
|
|
Thank you very much! That link is perfect; bookmarked; went from confused to "it makes sense". It implies "pocket" is what I'm looking for. It might be that Curve wasn't the trick, but it wouldn't generate an ops plan, forcing me to select "Contour mill", so maybe those issues where due to not using the right operation. Here's the latest using SolidWorks:  Compared to the script, the cuts are cleaner. Of note, there are several issues. I think at least some of them are due to post-processing: - I set the origin to the surface, bottom-left corner. When it goes to make the first move, it drags along the surface instead of going up some. If I can't work around this in solidworks, I could add a line at the start of the G-code manually to have it lift first. -It's not doing the circles right. Candle's throwing out Error 34 for "Invalid arc radius". I haven't yet dove in to see what's up exactly. - Near the end, it drives into the plastic (Left of the slot in pic) and jams. This isn't present in the SW or Candle simulations. Probably also a post-processing issue. Can narrow down the line where this happens with an air cut. edit: Confirmed the key to the type of cuts I'm doing is "Contour mill" operations, and from bbfu's list, Pocket is the feature type. Got it to sim correctly in SW using this. Dominoes fucked around with this message at 15:57 on Jun 13, 2021 |
|
#
?
Jun 13, 2021 15:46
|
|
|
Dominoes posted:Of note, there are several issues. I think at least some of them are due to post-processing: I'm begging you. Stop thinking that the output GCODE is something you should be editing by hand, ever. GRBL is a robust and well-supported output target for modern CAM packages. There should be literally no reason to ever open the .nc file in an editor to edit anything by hand, ever. The ability exists (as evidenced by the thousands of people who AREN'T editing their .nc files) to get your workflow set up properly so that the software and hardware are speaking the same language. GET YOUR POST PROCESSOR SET UP PROPERLY. Understand what it's doing. If you can't find the actual correct post-processor for GRBL in whatever CAM package SolidWorks is using, then find a different CAM package where there is a post processor speaking your exact GCODE language. The Shapeoko family of CNC routers uses GRBL; GRBL is a very robustly-supported output target. There is no reason not to set up your workflow properly RIGHT NOW so you're not embedding bad habits into your CUTTING MACHINE routine. Every time you say "the machine does x and I don't know why" is an opportunity to learn why. Is it something you're doing wrong in the toolpath setup (clearance heights, feed heights, safe retract height, etc) or is it something going wrong in the CAM -> GCODE translation? If you don't know, figure it out. When you do the toolpath simulation in SolidWorks, does it show the tool moving up and away from the material after moving to touch the surface when setting the origin? If not, why not? Should it be? Where does the simulation start the toolhead compared to where YOU start the toolhead when actually running the program? "Ooh the tool jams in the slot and drives away" would have already broken a tool and slung carbide shards around the shop if you had been working with a machine with actual power when cutting metal. Please please please stop thinking you can band-aid half-rear end solutions with hand-coding "fixes" when dealing with sharp spinning metal and actual stuff that can cause real physical damage.
|
|
#
?
Jun 13, 2021 17:01
|
|
|
Dominoes posted:Yes, slightly-modified to disable the coolant and tools, although these changes didn't seem to have an effect. Good to know! The way the Universal Post Generator works is that you start with a template and modify from there, and the M3AXIS one is an available options. I'll be working on it, but if you're inclined to poke around in the UPG, it's a starting point. Check your post settings, because you can disable coolant in the UI. If you right click a setup in the operation tree, select "Post Operation", you can insert an M01 break, and you can use that as an opportunity to change and re-zero tools if you're doing multiple tool programs.
|
|
#
?
Jun 13, 2021 17:14
|
|
|
https://nraynaud.github.io/webgcode/ Found this neat thing. It really points out where the origin is and what moves are happening in what mode. I was looking at my old code, and there aren't any positioning moves before the cutting starts. It looks like this: code:code:The first code was output with a python script plugin for Inkscape to cut flat shapes. The second code was created by Fusion360, an actual CAM package. The assumptions each package makes about where the machine starts is illustrative.
|
|
#
?
Jun 13, 2021 18:05
|
|
|
babyeatingpsychopath posted:I'm begging you. Stop thinking that the output GCODE is something you should be editing by hand, ever. This. Its important for your rapid prototyping speed, production processes and safety you get things right in your CAM setup such that you can be confident the output works as is. If you arent it will eventually lead to a big screw up, sometimes a dangerous one. (Learned this the hard way.)
|
|
#
?
Jun 14, 2021 01:39
|
|
|
Literally five seconds on Google and it looks like somebody else already solved this. http://www.restrictedayerspace.net/cnc/grbl-postprocessor-for-solidworks/ They even share their source files for the Universal Post Generator if you want to backtrack and make further customizations. The error in putting an asterisk at the start of comment lines that they mention can be solved with in a text editor with a simple Find-Replace command to replace * with a blank space (or just look through all of the places you can put comments in SolidCAM to make sure there isn't a stray asterisk somewhere). Some Pinko Commie fucked around with this message at 13:00 on Jun 14, 2021 |
|
#
?
Jun 14, 2021 12:58
|
|
|
It is also worth pointing out that everybody using SolidCAM/CAMWorks really needs to read the TechDB tutorials and learn how to go into it and customize it so that they don't keep having to make so many manual changes for safety-related things (NC retraction planes always being some distance above Top of Stock, etc.)
|
|
#
?
Jun 14, 2021 13:02
|
|
|
Thank you for the info and words of wisdom! I'm looking forward to going through that GRBL post processor, applying the new wisdom re coolant, tools etc, and see if I can get SW + the post-processor to make files that work directly (or almost work directly). Regrettably, I will be AFCNC until this evening or tomorrow. I've done some setup of tools and CNC machine in the Tech DB, but have a lot of work to do and experimentation to go there.
|
|
#
?
Jun 14, 2021 15:50
|
|
|
Dominoes posted:Thank you for the info and words of wisdom! I'm looking forward to going through that GRBL post processor, applying the new wisdom re coolant, tools etc, and see if I can get SW + the post-processor to make files that work directly (or almost work directly). Regrettably, I will be AFCNC until this evening or tomorrow. Did a bit more digging trying to find a post-processor for my hilarious toy machine (CNC Shark HD4) and found a GRBL post-processor for Solidworks CAM here: https://hawkridgesys.com/products/cam/post-processors/carbide-3d-shapeoko You end up signing up for some spam email in exchange for the post-processor, but that's a small price to pay since you can blacklist the sender once you get the post.
|
|
#
?
Jun 14, 2021 16:35
|
|
|
Let me know how that works - IIRC I couldn't get it working on non carbide machines using UGS. There has been a lot of drugs and alcohol between then and now, though 🤔
|
|
#
?
Jun 14, 2021 16:46
|
|
|
Awesome - going to try both.
|
|
#
?
Jun 14, 2021 16:59
|
|
|
|
| # ? Apr 26, 2024 00:58 |
|
|
Ayer GRBL postprocessor - works great! Had to remove one * line near the beginning, as mentioned. Going to make a few more of these, then try aluminum.
|
|
#
?
Jun 15, 2021 15:39
|
|