So like many others, I'm new and all of this is a learning curve.... I built my own CNC plasma machine using Openbuilds components. Current setup: - Blackbox X32 controller - OB Post Processor v1.0.41 - Fusion 360 for CAD/CAM - Currently 'fake the home' before shutting down - floating Z approx. 7.4mm before hitting Z probe I've had some successful cuts/parts and everytime it works...I feel like I've won a prize. But now I'm trying to really dive in and understand what's happening with the Gcode. While cutting something out yesterday, the plasma torch would scrap the work piece on its way to the first cut, but everything after that worked perfectly. That got me thinking about what I was doing wrong. So I started playing with settings in Fusion to see what I could change to fix that. One thing I realized in Gcode (attached), was the 'Pierce Height' was different from what I set it as in the 'Piercing' setting in the 'Linking Tab' in Fusion. After checking numerous things, I realized that in my Tool Library, I set the Cut Height and Pierce Heights to what my plasma manufacturer had recommended. As you can see in the Gcode and the attached screen shots, it looks like it ignores what I set in the 'Linking Tab' in Fusion, and uses what's in the Tool Library. I've tested this by changing the 'Linking Tab' to various numbers, but each time, the Gcode has what is set in the Tool Library. This seems to be different from other posts I've seen saying to put the Pierce Height in the 'Piercing' Tab. And as for the scrapping during the beginning of the job, I'm thinking now when I set the WCS to 0,0,0...I was putting the torch tip to almost touching the 'Stock Top'. And during the G53 move, it lowers the Z -.3937 (as I understand its supposed to do). SO by me putting the torch tip almost on the metal, first move is to lower Z, thereforce making contact and scrapping the work. SO I should set WCS with Z still up high in the same position as I home it...correct? Sorry for the long post...I'm trying to include all the stuff I normally see people not add up front.
I am going to reply to different things in different posts to help with clarity.... lets read that again.... on the linking tab is 'Pierce Clearance'. This is the HORIZONTAL distance from pierce point to start of cut. Pierce Height can be set in either of 2 places. a) as part of the tool setttings (best place) b) as a pierce height override in the postprocessor options this is preferred in the image below the 'pierce clearance' green line is pointed at by the purple arrow. Pierce Clearance sets the length of that move, which is primarily set the leadin/leadout distances
you mean SCRAPE, right? (which may well scrap the part as well as scraping along it (-: ) this is the result of an incorrect Z home setting, ie, you did not fake the home correctly and Z home is near the surface of the work. to recap faking the home: home is set when the blackbox powers up or is reset. move the machine by jogging to the correct home position (critical is Z HIGH at top of travel) reset the blackbox with the button on the side.
the primary setting for pierce Height is in the tool library. With the OB post you can override it in the post settings as indicated by the purple arrows. The green arrows reflect your settings for your probe offset
I have produced some gcode and am going to go through it step by step for you so you can understand the process. I would normally quote it as 'code' but that prevents me from adding comments in color (red are my comments). Also make sure you have read OpenBuilds-Fusion360-Postprocessor/README-plasma.md at master · OpenBuilds/OpenBuilds-Fusion360-Postprocessor (Made in : Autodesk CAM Post Processor) (G-Code optimized for Grbl 1.1 / BlackBox controller) (OpenBuilds CNC : GRBL/BlackBox) (Post-Processor : OpenbuildsFusion360PostGrbl.cps V1.0.42) make sure you have the latest version! (Units = mm) (Laser UseZ = false) (Laser UsePierce = false) (Arcs are limited to the XY plane: if you want vertical arcs then) (edit allowedCircularPlanes in the CPS file) (Drawing name : Water-Laser-Plasma v2) (Program Name : plasma) (1 Operation (1 : Through-medium quality_left-Comp) ( Work Coordinate System : G54) ( Tool 3: Plasma Cutter Diam = 4mm) ( Machining time : 0h:0m:19s) G90 G94 G17 moves will be in absolute coordinates on the XY plane G21 (Plasma pierce height 0.77) as overridden in the post settings (Plasma topHeight 0.1) this is the cutting height set as 0.1mm from stock top in the 'top height' settign in the 'heights' tab (Operation 1 of 1 : Through-medium quality_left-Comp) G54 (Plasma cutting with GRBL.) (Using torch height probe and pierce delay.) (This relies on homing, see Search Results for Query: G53 fusion | OpenBuilds ) G53 G0 Z-10 move to -10mm from the Z HOME position, Z home must be top of travel G0 X127.207 Y142.667 F1000 G0 X127.207 Y142.667 Z15 come down to 15mm above the material, 0 begin set by your setting of WCS Z=0, and will be refined by probing G38.2 Z-30 F100 probe G10 L20 Z-7.4 set offset G0 X127.207 Y142.667 ; force position after probe Z0.77 move to pierce height M3 S1000 plasma on G4 P1.8 pierce delay as set by the 'spindle on/off delay' in the post properties G1 Z0.1 F1000 move to cut height G1 X128.187 Y142.472 start cutting X128.325 Y142.714 X128.448 Y142.964
This is perfect and clears up my confusion! Thank you for taking the time explaining with screenshots. I have read so many different posts of similar-ish topics...I confused myself.
Yes, I meant SCRAPE. I believe now what I did was after I powered on my machine (with it homed as recommended), I initially scraped the work and I manually "alarmed" the job since it was scraping. After that, I cleared the alarm manually, but did not re-home. Does manually triggering an alarm, then manually clearing it cause it to lose MCS Home? I have an EPO switch but havent installed it yet. Other than that question, I understand the importance of correct homing prior to shutting down! Thank you again.
I'm tracking on this too now! I saw that the override Pierce Height in the Post is another option to set Pierce Height. I'll continue to use my Tool Library but keep this feature in mind. It's nice having it in multiple places....once you figure it out lol.
This is awesome! Before I made this post, I googled all these commands to "see" what was going on and I'm happy to see that my notes match yours....WIN! This explanation is perfect for someone like me and I'm sure it'll help others in my same situation. Thanks again for taking the time to answer all my questions...and break it up for clarification too. You guys rock here at the OB team!
I am new also but aft reading your post now I am really confused. Everything I read says cutting height 1.5mm, Pierce height 3.8mm Clearance height 10 mm and using "G10 L20 Z-7.4 set offset" I use the Z-7.4 number to fiscally set the Cutting height, material face to torch tip face with feeler gauges to hit my 1.5mm cutting height. Why are my numbers wrong. I am going to read your post a few times,just to let it set in. A explanation like this is what I think all of us new people need on a few different subjects line by line with a explanation from the person who wrote the Fusion up date. Between bad and old information I don't know what to believe. I have read posts from all you guys some of them are the same over and over this would maybe even help you. If this is out there I haven't found, just in case Peter reads this and alI of my questions are posted in a link somewhere just kiding. I think I get it but my numbers are wrong I keep fighting different things most I don't know and it takes for ever to fine the correct answer. My wife has seen so many YouTube videos I bet she could run something through Fusion cam. while I have you I am also trying to get a better transition from the tool path to cutting face, I have tried different lead in/out settings but nothing seems to work good enough. what is the best I can expect to achieve so I can move on to some of my other problems. Thanks for you time and help Maybe my brain is just getting to old for this, whats that saying old dog new tricks. Ok I wasn't 100% on Pierce Clearance. I'll try working with that.
set this as the offset from 'material top' in the top height setting in the heights tab. the surface of the material is Z=0. This is set this way because when the post was first written there was no value in the tool definition for cut height. I will be changing the post to use the tool value if this offset is 0. set this in the tool definition and then do not override it in the post options set this in the heights tab this is set by the probing to find the surface of the material "here where I am going to start cutting" . This is because the sheet of metal tends to bend from the heat during cutting, so each start point is re-probed to account for most of the bend. The value must be the difference between 'torch tip at surface of (flat) metal" and where the probe switch trips when the Z moves down and the torch tip is pressed against the metal and moves up. I was having mixed results the other day when I was playing with this. sometimes Pierce Clearance makes a difference, sometimes not. Both the 'lead-in/out' value and the 'pierce clearance' value will affect how far away from the cut line the cut is started (in fusion help), but pierce clearance appears to be overridden by lead-in/lead-out if those are defined (and maybe some other options also change how it works). I would stick to defining the lead-in/lead-out values and ignore Pierce clearance.
Lol, man I am in the same boat as you are. It can definitely be discouraging, but one thing that helped me it to keep making mistakes here and there...each time you either figure something out, or plant the seed to figuring something out. I found some inconsistencies between what popular posts on this issue were saying...and what Fusion actually had in CAM. It took me correlating small things here and there to finally figure it out. Yea once us new guys see numbers from someone else...it's all over lol. Theres really only 3 numbers I focus on in the CAM/POST.... 1. Z OFFSET: if you are using the Touch Off Probe (I do and mine happens to be 7.4mm). What helped me is put a piece of metal plate down on your table and run your Z axis down slowly until it just makes contact with the metal plate. Now Zero Out the Work Coordinate System (Zero All button in OB Control). Then slowly continue to lower your Z axis until you see your Z Probe switch light up. Observe the negative Z number in OB Control and enter that number into your Post Processor settings in Fusion 360. Do this check a few times to make sure you are getting the same numbers. 2. CUTTING HEIGHT: As David said, this number should come from your plasma cutter manual and it's entered into Fusion in the "HEIGHTS TAB" (Pic uploaded) 3. PIERCE HEIGHT: This confused me too. This number is pulled from your TOOL LIBRARY in Fusion (Pic uploaded mine is 0.1 inch). When you setup a tool, it's stored locally or in the cloud depending on where you saved it. If you open up your Gcode, it will define the PIERCE HEIGHT. I thought this number was supposed to go into the LINKING tab in Fusion, but it does not. Nah man....our only limitations are ourselves. People go to school for this kind of stuff! We just use Youtube, forums, tears, etc! You will figure it out in time...and once that lightbulb turns on (which is the reason for my original post), you'll be able to visualize things as you are setting up Fusion/Post and it will be so much clearer.
