|
Edited for quoting since the reply ended up starting a new pageDominoes posted:Ayer GRBL postprocessor - works great! Had to remove one * line near the beginning, as mentioned. If it wasn't for being  I'd ask if someone could put that post processor for GRBL on a file sharing site and post a link here for everyone else looking to experiment with SolidCAM and their Shapeoko/GRBL machine.EDIT #2: Make sure you recalculate your speeds/feeds and depths of cut/stepovers for aluminum, since I'm sure it will require a much lighter touch. Some Pinko Commie fucked around with this message at 16:05 on Jun 15, 2021 |
#
?
Jun 15, 2021 16:03
|
|
|
|
| # ? Apr 27, 2024 01:56 |
|
|
It was the restrictedayerspace.net link you posted earlier. Good call on aluminum. Of note, the speed (S setting) here was too high for the 3018, but in the case its commanded to a speed higher than its max of 1000, it goes to 1000.
|
|
#
?
Jun 15, 2021 16:07
|
|
|
Dominoes posted:It was the restrictedayerspace.net link you posted earlier. I know, I meant for folks that don't want to sign up for spam email to get it. Have you played around with choosing "Library" for the Feed/Speed tab and then using the Stock Manager to set the material to something like what you are going to machine? If you pick, for example, 6061 (maybe the most common grade of aluminum people machine?) in the Material under the Stock Manager, then the software will take a guess at the appropriate spindle and feed rates to use under the Feed/Speed tab as long as you have "Library" picked and have set the material in said stock manager. This can be handy if you're experimenting and want relative starting point feeds/speeds to then adjust from with your overrides on the machine (usually a dial for the RPM and a dial for the linear feed that's in percentages--but this may vary depending on your machine). There is a weird/painful process for enabling more material options in the TechDB (or at least, it was painful when I last did it circa 2018), but I figure more baseline data is a good thing when you're starting out (and you can always change the Feed/Speed option to Operation and put your own feeds/speeds in if you don't like the Library's guesstimate). Some Pinko Commie fucked around with this message at 16:34 on Jun 15, 2021 |
|
#
?
Jun 15, 2021 16:31
|
|
|
I used the non-spam one. I set up the spam one too and skimmed the NC files it generates (about 2x longer than the Ayer and FANUC ones) For the Feed/Speed tab, I've left default settings of Library, and used Polyurethane for the cut above. There are a few aluminum setting there too, including what it defaults to (I think the 6061 you mentioned? I'll use that when I try Al). I was surprised that selection is so small - eg there wasn't an ABS setting. On the materials setting for the CAD part of SW, there's a much larger material library, but it seems independent from this. I may try the Operation setting and experimenting, especially if the default Aluminum doesn't work. Or if sending 10000 RPM to the machine that can only do 1000 (and reverts to it) messes with the feed/drill speed ratio or something.
|
|
#
?
Jun 15, 2021 16:44
|
|
|
Dominoes posted:I used the non-spam one. I set up the spam one too and skimmed the NC files it generates (about 2x longer than the Ayer and FANUC ones) Yeah, the CAM material library is completely separate from the SW material library (for the simple reason that the feed and speed tables mean nothing to Solidworks yet, and they haven't really integrated the software yet to the point that the same material library could be used for both). Here's a "quick" walkthrough of how to add more materials to your list (and you can go through the list of available materials and pick materials you are likely to attempt to machine and remove materials you know you never want to mess with). https://hawkridgesys.com/kb/add-camworks-stock-material-in-technology-database
|
|
#
?
Jun 15, 2021 16:55
|
|
|
Nice! I'll dive into that if the Aluminum settings don't work, or maybe to get a proper ABS. Another note: It appears the Ayer post processer is skipping a drill step I have at the end that the Hawkridge (spammy one) works with.
|
|
#
?
Jun 15, 2021 20:35
|
|
|
I'd wager the Hawkridge one is going to be more well-defined and you're going to end up having more reliable code output there (since it's from a business that uses it as a "come to us for a post-processor for your other CNC needs" lure) vs. the Ayer post processor being done by a self-admitted amateur.
|
|
#
?
Jun 15, 2021 21:14
|
|
|
Did the Ayer one use a canned cycle? Probably G80-something? I don't believe GRBL supports ANY canned cycles
|
|
#
?
Jun 15, 2021 21:17
|
|
|
Nailed it. G80. Need to get some sacrificial plywood and smaller t-rail clamps before trying the aluminum.
|
|
#
?
Jun 15, 2021 21:39
|
|
|
NewFatMike posted:Did the Ayer one use a canned cycle? Probably G80-something? I don't believe GRBL supports ANY canned cycles Could also go into the TechDB and disable canned cycle output on that side of the software (force the post to output long code for each movement). We did that for one of the machines at work because, while it did support canned cycles, once you had a part that had more than about 30,000 holes the drip-feed code lost the canned parameters (& then the machine would just rapid to each hole location but not actually perform the drill function, serious WTF moment). Some Pinko Commie fucked around with this message at 23:47 on Jun 15, 2021 |
|
#
?
Jun 15, 2021 23:44
|
|
|
Ooh, that's... Fun. Since it's in the past, I guess. I never knew you could disable canned cycles in the TechDB, that's very good to know from a post processor troubleshooting side. Dominoes posted:Nailed it. G80. 
|
|
#
?
Jun 16, 2021 05:16
|
|
|
biracial bear for uncut posted:Could also go into the TechDB and disable canned cycle output on that side of the software (force the post to output long code for each movement). Ahh
|
|
#
?
Jun 16, 2021 12:37
|
|
|
NewFatMike posted:Ooh, that's... Fun. Since it's in the past, I guess. Yep. You have select your machine then go into the operation parameters for your various drill cycles to disable it as needed. But doing this for something like your variable-pecking cycle when your machine might not otherwise support it is handy.  CarForumPoster posted:Ahh The machine in question was built by Anderson America (their Stratos line of machines) and set up new in 2005, but yes. Weird configuration using a Windows PC that emulates FANUC software instead of having a proper FANUC controller setup. I hate it.
|
|
#
?
Jun 16, 2021 12:53
|
|
|
Is every controller that lives on a timeshare OS terrible, or are there any good ones? Because Mach, GRBL, and ShopBot are ones I've tried and they are not fun compared even to PathPilot.
|
|
#
?
Jun 16, 2021 13:27
|
|
|
I'm pretty sure they are all terrible. I briefly (through 2019) worked for a company that had HAAS machines (plus some routers that also had direct FANUC controllers on them, but I can't remember the manufacturer's name) and those things ran pretty much flawlessly with whatever code options I threw at them. Canned cycles, subroutines/programs, even some limited macro logic statements to generate hole patterns and slots/etc. based on variable values that the operator would input in a file they would edit for the variables required before running the program. I wish I could afford to dump some money into a HAAS TM-1 with some of the add-ons that are available for it (tool probing system, "convenience package" for the tool/clamp/etc. storage, "High Speed Machining" and Rigid Tapping) , and be able to just Make Stuff.
|
|
#
?
Jun 16, 2021 13:43
|
|
|
GRBL runs on an 8-bit Arduino, which is simultaneously incredible, and why its terrible.NewFatMike posted:Is every controller that lives on a timeshare OS terrible, or are there any good ones? Because Mach, GRBL, and ShopBot are ones I've tried and they are not fun compared even to PathPilot.
|
|
#
?
Jun 16, 2021 13:49
|
|
|
biracial bear for uncut posted:I'm pretty sure they are all terrible. One day we'll make it! LightRailTycoon posted:GRBL runs on an 8-bit Arduino, which is simultaneously incredible, and why its terrible. Oh yeah, they all need to be fed by UGS and things like that, too. I still haven't set my 3018 up for GRBL from Mach 3, but I do have the offline controller, which I forgot about. I've had better experiences with GRBL than Mach 3 which is bananas in its own way.
|
|
#
?
Jun 16, 2021 14:17
|
|
|
I actually like the "CNC Shark HD4" control setup (reminds me of a scaled-down version of the old dinosaur Thermwood my employer used to have with it's manual spindle dial to control RPM, no tool library, and no tool touch-off that stores tool offset value for the current tool). Really wish I had a way to do a good semi-automated touch-off though. The stupid pendant that came with the machine for that purpose doesn't work at all (and a replacement is $100? When I have no guarantee it'll work at all?) Some Pinko Commie fucked around with this message at 14:30 on Jun 16, 2021 |
|
#
?
Jun 16, 2021 14:19
|
|
|
Gotcha on the Hawkridge GRBL for machines like the 3018: It inserts a G28 near the beginning, which rapidly moves to the machines 0 coords. If you're used to working in work coords, this can have consequences! (Of note, I haven't found a way to center the machine coords, so have been removing this line)
|
|
#
?
Jun 17, 2021 13:48
|
|
|
Dominoes posted:Gotcha on the Hawkridge GRBL for machines like the 3018: It inserts a G28 near the beginning, which rapidly moves to the machines 0 coords. If you're used to working in work coords, this can have consequences! (Of note, I haven't found a way to center the machine coords, so have been removing this line) In between powering up and running the program, can you not jog the machine to your safe position and reset X/Y/Z to be that position with regard to G28 (assuming the machine in question doesn't have homing switches)? Another option would be to put some X/Y/Z values after the G28 that you know will be safe relative to your actual setup. Like "G28 Z5.0" (or any other arbitrary Z-value that would be a safe distance above your setup without causing overtravel) will just have the machine move the Z-axis to what it thinks is Z5.0 above "Z-home" position and X/Y would remain wherever the machine currently is because G28 plus an axis callout only moves that specific axis. EDIT: That could still be a problem depending on the controller because some machines will interpret "G28 Z5.0" as "Go to Z5.0 relative to machine Zero on Z-axis" and some machines will interpret it as "Home Z-axis, then go to Z5.0". Some Pinko Commie fucked around with this message at 14:48 on Jun 17, 2021 |
|
#
?
Jun 17, 2021 14:44
|
|
|
I appreciate it! The machine coords sound useful, but I'm not sure how to sync them or make them meaningful, since there are not sensors, stops etc, or any way to measure Them. And if I plug the machine to usb but not wall power, eg to simulate, the machine coords move without the machine moving, so it seems useless. When G28 runs, it tries to send the machine way out of limits.
|
|
#
?
Jun 17, 2021 19:06
|
|
|
First thing I would do, is look for a guide on how to add endstops to your machine so that it reads and interprets homing actions correctly (since the firmware clearly has support for it enabled, but the hardware on your machine just isn't available for it to run properly). EDIT: Like this one: https://samueldperry.com/2020/09/01/cnc-3018-pro-router-adding-endstops/ EDIT #2: Found one that may be less bullshit to implement. https://docs.sainsmart.com/article/rerey17twl-adding-axis-limit-and-emergency-stop-switches-to-a-sain-smart-3018-pro-cnc-machine Some Pinko Commie fucked around with this message at 19:31 on Jun 17, 2021 |
|
#
?
Jun 17, 2021 19:22
|
|
|
Oh sweet!
|
|
#
?
Jun 17, 2021 20:36
|
|
|
The only reason I ever edit gcode directly is when I have a swivel knife loaded instead of a cutting tool and gotta delete the line that starts the spindle---M3, in my case. This is an incredibly specific situation and if my workplace invested in newer software I don't think I'd need to do it.
|
|
#
?
Jun 18, 2021 03:58
|
|
|
Trebuchet King posted:The only reason I ever edit gcode directly is when I have a swivel knife loaded instead of a cutting tool and gotta delete the line that starts the spindle---M3, in my case. This is an incredibly specific situation and if my workplace invested in newer software I don't think I'd need to do it. How much money was invested in the post-processor development (assuming you ever got to see the purchase orders)? That isn't free, despite what Autodesk might have people believe after they dumped the post-processors from HSMWorks into Fusion (back when they bought all the rights to that software and got access to the code and post-processor archives). EDIT: HSMExpress is an option for Solidworks if you're sticking to 2.5-Axis operations and want to play around with an alternative to CAMWorks/SolidworksCAM. They also have a GRBL post-processor for download. Here is where to download HSMExpress: https://www.autodesk.in/campaigns/hsmxpress-download And you can run a search for post-processors here: https://cam.autodesk.com/hsmposts Just select "Milling" for post Type and then select "GRBL" for the vendor. EDIT2: Holy LOL there is a post-processor for a MaslowCNC if anybody wants to build one of those and start loving around. Also! The post-processors are Javascript-based, so if you have an editor that will open Javascript files (Notepad++ or any other text editor that isn't an Office or Office-like product will work), you can dig into the post-processor's guts and customize things more easily. Some Pinko Commie fucked around with this message at 11:07 on Jun 18, 2021 |
|
#
?
Jun 18, 2021 10:57
|
|
|
biracial bear for uncut posted:How much money was invested in the post-processor development (assuming you ever got to see the purchase orders)? https://marketplace.visualstudio.com/items?itemName=Autodesk.hsm-post-processor Start here and use visual studio code to edit your post. You can set it up so your post and the gcode it creates are aide by side. Click the g code and it will highlight where in the post it came from.
|
|
#
?
Jun 18, 2021 12:33
|
|
|
honda whisperer posted:https://marketplace.visualstudio.com/items?itemName=Autodesk.hsm-post-processor Nice! Here is the main application you need to use that add-on, other folks in the thread that may not have Visual Studio Code: https://code.visualstudio.com/ EDIT: I figure I'll set it up and play around with it for the Anderson America postprocessors for HSMExpress; it'd be nice to have an alternative to SolidCAM/CAMworks for when the employer decides to pour-mouth about updating software and things start breaking again.
|
|
#
?
Jun 18, 2021 12:47
|
|
|
I had been interested in the Silhouette Cameo 4 Pro for some projects, especially textiles, and I got a job that was a good opportunity to pick one up, so I did, and about a week later, I'm returning it. I'm really sad because I really thought it was cool, but this thing skews tremendously and by spec has an error of 65 thou per foot. Like what the gently caress? How is that usable for any professional application? It can't even close an 18" x 18" square it skews so much. I guess I get to be That Guy™️ this week at the makerspace and just monopolize the lasers. E: it's a shame the Ortur Laser Master 2 couldn't get here by the deadline - anyone know what kind of acrylic/plastic I would need to enclose it? NewFatMike fucked around with this message at 00:20 on Jun 20, 2021 |
|
#
?
Jun 20, 2021 00:05
|
|
|
You probably know this, but don't use the laser for vinyl
|
|
#
?
Jun 20, 2021 00:38
|
|
|
Oh yeah, vinyl was none of the things I was going to use any of these for
|
|
#
?
Jun 20, 2021 00:49
|
|
|
So here's a weird one. Job shop, just got a 600 piece order. Normally we make 1-4 parts at a time. It's a rectangle 2x8x1.25" with some features. Customer supplied 3d models. It's 3 different parts, and other people set them up on 3 different hurcos. First op, on all 3 parts, they came out 2.002"x7.998" Checked the models, they're good and square. Gcode looked good, centered in the middle and it came out 4.25 in x and 1.25 in y programmed on tool center so should be good. I get drug in to try and figure out wtf. Checked everything I could think of. Out of frustration just made my own model, posted it.... And its perfect. Copy pasted tool paths, feeds, speeds, everything. Even compared the code 1v1 and they're identical. Fusion 360 for the software. What the hell.
|
|
#
?
Jun 24, 2021 01:42
|
|
|
Did you check the actual tooling? Also is +/-.002" enough to reject the part? When was the last time the machines were serviced? Because that sounds like either wear-based backlash starting to creep in (& setting up in a different position on both axes would temporarily relieve that) or somebody hosed the initial setup and is covering tracks. Also I'm not familiar with Hurco machines, but there is also a chance that a modal comp code may have still been in memory if the operator didn't clear memory before loading the new program/setup. Ran into that once at a shop I used to work at because some weird firmware setup allowed that even after M02. Literally had to make sure the starting Gcode had all applicable G/M-codes required to reset comps/etc. to off before the first tool callup. Some Pinko Commie fucked around with this message at 01:55 on Jun 24, 2021 |
|
#
?
Jun 24, 2021 01:48
|
|
|
It's kinda weird that it's the same on all three machines, that suggests against backlash and other machine issues in my mind. Is it the same 1/2" endmill assembly on all three machines? Did you get a batch of reground tools in (or buy a bunch of bargain-bin rejects)? Or, if you're actually using cutter comp, recalibrate your tool probes/presetter recently? (And even if you're not intending to use cutter comp, check the programs to make sure that there aren't any G41/G42/Hurco-equivalent commands in there.) Alternatively, could it be tool deflection? If you've got identical tool setups and the spindles are very similar that could repeat pretty well between machines. 2 thou would be a decent amount of surface location error for a 1/2" cutter, but not impossible, depending on how much tool extension you have. How much stock are you leaving for your finish pass? EDIT: Read a bit more carefully. It'd only be 1 thou of deflection on each side, which is pretty reasonable, but it's interesting that one side is long and the other side is short, that suggests against cutter comp issues as well. Are those dimensions consistent across the entire length of the part? Karia fucked around with this message at 02:12 on Jun 24, 2021 |
|
#
?
Jun 24, 2021 02:08
|
|
|
Milling direction (climb vs. conventional) and tool stick out between setups could be an issue, too.
|
|
#
?
Jun 24, 2021 02:14
|
|
|
biracial bear for uncut posted:Did you check the actual tooling? No cutter comp in the gcode, checked the machines anyway and they're zeroed as well. The people who did the initial setup already called the service guys in and they said everything was perfect. One older machine, one a couple years old, and one about 6 months. Also checked and no skew value in the setup. +/-.002 won't kill the part but it makes the next ops a pain because other features call back to those edges. Karia posted:It's kinda weird that it's the same on all three machines, that suggests against backlash and other machine issues in my mind. Is it the same 1/2" endmill assembly on all three machines? Did you get a batch of reground tools in (or buy a bunch of bargain-bin rejects)? Or, if you're actually using cutter comp, recalibrate your tool probes/presetter recently? (And even if you're not intending to use cutter comp, check the programs to make sure that there aren't any G41/G42/Hurco-equivalent commands in there.) It's consistent for the whole length. New tooling in good holders. I checked the runout myself and it's .0001-.0002" I don't know what they left for the finish passes but it does have an extra flex pass baked in. I checked it for deflection and it's miniscule. That it's long one way and short the other has us all confused too. These machines are super consistent. We know which ones can hold tight tolerances and which ones are clapped out. None of these are the clapped out ones. Outside this one job you tell any of them to mill that same shape and it would be 8.002x2.002 to 8.001x2.001. Our endmills are almost always .499-.498. Mic, offset, send it. If been staring at it a long long time before I finally said gently caress it the only common factor is the models. Let's make our own to rule that out. I'd even taken multiple material samples and checked their hardness to make sure it was consistent. 4140pht all 29-30 Rockwell.
|
|
#
?
Jun 24, 2021 02:42
|
|
|
 Sounds like you've got your head on straight about what you're checking. Vise squish was my other guess, but running the numbers on that for a 1.25" tall block of 4140 seems like it'd be way less than a thou. New tooling doesn't always mean much, but given the specific error you're seeing that doesn't seem like the problem. Last guess before I stop playing backseat machinist for the evening: I'm sure you've already checked it, but is your measuring equipment OK? Nobody dropped your 2" mics, right?
|
|
#
?
Jun 24, 2021 03:10
|
|
|
Karia posted:
Way to chunky of parts to be deflection from the vise pressure but good thought. As for measuring I brought mics over to make sure and took a part to inspection to confirm. Also you're not being a backseat machinist, I asked here for a reason. I'm looking for the blind spot I'm missing.
|
|
#
?
Jun 24, 2021 03:17
|
|
|
Compare the actual g code between the two! You can probably see something glaring like it deciding to run the tool in a rectangle .002 too small.
|
|
#
?
Jun 24, 2021 03:40
|
|
|
Commodore_64 posted:Compare the actual g code between the two! You can probably see something glaring like it deciding to run the tool in a rectangle .002 too small. I did. That's what's really breaking my brain. They are as far as I can tell identical. At least the finish pass. Before I left we were debating calling ghost hunters vs laying out a pentagram with dykem and having an exorcism. I'll check it again tomorrow and post the gcode. And see if it works on the other machines.
|
|
#
?
Jun 24, 2021 04:16
|
|
|
|
| # ? Apr 27, 2024 01:56 |
|
|
Last thought before going to bed: stress relieving causing the part to distort? It'd be weird to have that just make the part smaller and not bow it since you're presumably only doing one face in this operation, but internal stresses can do seriously wacky stuff, and could absolutely cause the part to shrink in only one direction. Try mic'ing the dimmensions immediately after they're cut (allow time to cool down to 68F if necessary, of course.) If that looks OK, then try shifting the finish pass to the very end of the program if it's not already there and see if that changes anything (not just the spring pass! Spring passes don't do anything if the material's already shrunk, obviously.)
|
|
#
?
Jun 24, 2021 04:47
|
|