Hi All... So I have built my new CNC machine - YAY I drew a picture with a sharpy - YAY I tried milling out a basic square drinks coaster drawn in fusion 360. I generated the G-Code however some issues then occurs. I loaded the Gcode into my Duet controller. I set the work zero - and the coordinates change on the webpage. When I run the g-code from Fusion360 a simple 2D facing operation the machine move rapidly moves to 0,0 of the machine, and then plunges the Z xis down. When I inspected the G-Code I executed line by line to try and see what was happening - Most commands are not supported as they are tool selection. - Then the command appears G54 - When I execute this the coordinates shown in the top corner revert back to the machine coordinates, meaning the next the command to run setting the X and Y are referenced from the machine 0,0 rather the work 0,0. Can anyone help? Something related maybe be when I hit the pause button the Z axies plunges into the workpiece then goes up, the x and y move a bit back and forth then all stays still. The movement buttons do not step the usual distance, much bigger distances. I have disabled G28 Safe retracts if that makes a difference? Home this all makes sense, G Code attached for the face operation. Happy to share access to the model in Fusion of that would make it easier to help with? Regards Colin.
I am using fusion 360 with the post processor written by Oozenest and have no problems. Which post processor are you using? Alex.
Also have you disabled "allow moves without homing" and homed all axes when you switched the machine on. How familiar are you with fusion 360? It sounds as though there is confusion about which axis is which. Alex
Go to Oozenest, search for fusion 360 post processor, go to workbee firmware updates, download latest version of fusion 360 post processor. Can't remember how I got fusion 360 to use it, but there are instructions in fusion. If you have difficulty with this message me and I will look it up tomorrow. Alex
Link to the latest oozenest fusion post: https://ooznest.co.uk/wp-content/uploads/2019/02/Fusion-v1.0.1.zip How to use a custom post: How to add a Post Processor to your Personal Posts in Fusion 360 | Fusion 360 | Autodesk Knowledge Network
No worries. Colin. If you still have issues after using the oozenest post, please let us know where you are setting your origin.
Hi Alex Cheers - Just tested and and all cutting in teh right place!!!! FYI anyone else reading this post use mm not inches. I saw a video once say inches should be used .. not with this post processor!!! once again - THANK YOU!!!!
Sorry Sharmstr I was in the garage testing it all out... the Good news.. its all working now I need to get my head around all the CAM stuff. @Alex thank you!! Now I have just realised the time... back to the real world of work tomorrow!!! :-(
Look into creating CAM templates. Also, since I'm American, I find its easier to model in imperial, but cam in metric. I have cam templates for my most common types of materials, bits and toolpaths so I rarely need to worry about metric when I'm applying toolpaths. I just import the template I want, select the correct geometry and its done. To measure my stock I use a keychain size tape measure that has both imperial and metric. If you need fusion help, hit us up.
Hi @Colin Hart One thing I've learnt on this build is problems no mater how small are always going to creep up and have to be solved (aint that just life lol) You've come a long way, a lot faster than me...I went a different route for the software CAD/CAM side of things in VECTRIC.. purely because it seemed a simplier GUI especially for a newbie as myself to get their head around...All that said...and no matter what folks are using to achieve a common goal, would you be so kind as to post up images of your first attempts at milling, (dont worry I'll be doing likewise) material choice, size of bit, speeds, and any other relevant data for the process......Just to gauge what can be expected from this machine (from birth if you like)..You say you are trying to mill a simple drinks coaster, once you get the post processor thing sorted out and try again, Would you say your pleased with your efforts, does the piece need much finishing i.e. sanding etc are there things (cad/cam) you could tweak to improve the piece. Did you surface your spoilerboard, what milling bit did you use?? Sorry for the inquisition atb C
Hi @sharmstr, I'm old and British, so I am happy working in either imperial or metric - in fact I have been known to mix the two - larger numbers in imperial and smaller ones in metric. I am a newbie to cad/cam though and haven't heard of cam templates could you please enlighten me or point me to somewhere I can find out more? Alex
I'm old too so we have that in common There's a lot of resources out there, but two that I would recommend is John over at NYC CNC and Lars Christensen. While they probably dont have videos specifically targeted at cnc router users, I'm sure you can still learn a lot from both of them. Here's some videos I suggest. Some are a few years old so some things may have changed a bit, but it will get your started.
No problem. It really is. It took me a bit to get them setup and tested on the machine, but once its done you can fly through new jobs.
@sharmstr- Awsome links. So I have daft question and this is probably the wrong place to post but it does follow the theme of #NewbieQuestions, and #SteapLearningCurve. I am preparing my CAM in Fusion 360 - (I had a list of guitar parts I wanted to work on, however, my 7-year-old son had other plans. I present article 1: Harry Potter! a 10 x 10 wood thing. I have created 2 CAM jobs so far: 1. 2D Adaptive Clear - 6mm 4 flute, straight end mill. This is fairly straight forward. As you can see a fairly rough tool path clearing out much waste!! 2. I then switch to a finer bit, however rather than taking into account the material removed from the previous process F36 has decided to remove stock that isn't there. I feel that I must be doing something total wrong, and "justified comments" are permitted. Cheers all for reading from a middleaged Brit (who is going grey fast) Regards Colin.
Not a daft question. ( i believe that's the first time I've used the word daft without punk after it) Anyhow, you are looking for "Rest Machining". Its not available in 2D adaptive. Switch to 3D adaptive and select Rest Machining from Previous Operation. There's also "both ways" machining in the passes tab. Do a youtube search on it and see if you want to use it. It will allow you to use both climb and conventional cutting thereby reducing your run time. Again, watch a video or two on it because there are some gotchas!
Hi Colin, I am a complete beginner on Fusion 360, but I tried something similar to your project. Setup with 20 mm stock side offset, 6 mm tool, adaptive clearing, leave stock 0.5 mm I got the following toolpath Setup 2 stock side offset 0.5 mm, 1 mm tool, 2d contour, and got the following toolpath I don't know the details of your project (eg stock thickness) so I didn't bother with multiple passes or setting depth of cut, but I suspect your underlying problem may be that you didn't do a separate setup for the finishing cut. Like I said I am a beginner, so this is not a definitive answer, but it might steer you towards a solution. Please let me know what the outcome is. Alex
Hi Alex. That's a good strategy. But if you look at the details of his model, the 2d contour might not get all the stock. As you say, its something he'll need to figure out. The good thing is that rest machining will only get the bits the bigger bit couldnt reach, then he can do the 2d contour as a finish pass.
Hey Alex.. this is interesting, i'll have a play over the weekend. The 3D tool paths do seem to do the trick to a degree.
Hi Colin, I have had a further play - @sharmstr was posting her response as I was composing mine. I think you need to read both responses @sharmstr is right about using rest machining AND you need two separate setups. My response suggested using 2d contour as the finishing toolpath, but this could miss some bits that the first roughing pass hadn't removed. Have fun and let us know how you get on. Alex
Side note. You dont have to make multiple setups, even if you change tools. Instead of selecting "Setup" when you post, just select the toolpath(s). Lets say the first toolpath uses a 1/4" endmill and the 2nd and 3rd toolpaths use an 1/8". Just select the first toolpath and then post process. Then select the 2nd toolpath, hold down ctrl and select the 3rd toolpath then post those to a different file. Edit: This comes in real handy when you want to use rest machining since I have found its better to have it know about the previous operations. It doesnt if you have different setups. When I get some spare time, I'm going to modify the post processor to automatically create separate .nc files for each tool change.
Thanks @sharmstr. Which post processor though? Colin and I are using the Duet controller which uses Reprap firmware - not Grbl. Alex.
I'll be modifying the grbl based post for my needs if that's what you're asking. Though I looked at the Oozenest post and its not really that different. Looks like it was originally based of the grbl post. The ability to post toolpath(s) within a single setup is not post specific. So my advice is valid for you guys.
Thanks @Colin Hart for posting your cam problem, I think I have learn't more from looking at that and @sharmstr's tips than I have in hours of trying to work through tutorials. Alex
