Can you use fusion 360 without preset tools?

18 Mar 2017 19:11 #89865 by Dougefresh
Im having a hard time finding Information on how to configure cnc linux with fusion 360 without preset tools, any help or direction would be greatly appreciate. Im using an old den ford micromill and it came with an 1/8th inch collet that seems to work ok with Dremel bits, ( all I have that are easily obtainable). Ive been reading orangecats posts on how he has set up linux cnc to program a pause to change his tools mid program. Im just wandering if fusion 360 would work with this type of manual tool change and how other go about it. Im a total noob but I have high hopes that I will eventually get this figured out. worse case scenario I will be forced to just buy a bunch of tool holders and move forward. Also at this point I have a good concept of how most things in linux cnc work together but am a little stuck on how to correctly modify my hal file for orange cats manual tool change.. everything else seams pretty straight forward.
19 Mar 2017 01:07 - 19 Mar 2017 01:12 #89872 by kornphlake79
The best thing to do is create a program for each tool. There isn't any provision in linuxcnc to touch off tools between tool changes while a program is running, without some kind of tool holder you have to touch off the tool manually with every tool change because the tool length changes unpredictably with every tool change. It really isn't that big of an inconvenience running the machine, but it is a little tedious to have to post each tool path individually in fusion360
Last edit: 19 Mar 2017 01:12 by kornphlake79.
19 Mar 2017 18:43 #89894 by Dougefresh
Thanks kornphlake, I was thinking that would be the only way... So do you just make multiple copies of your part In fusion and then If you have three tools you would just save three individual files with only one tool path per file? I seems to me that you would run a tool path with your first tool ( the one that has your offset and diameter in the linux cnc tool table) and making sure it corresponds with the same tool created or selected in fusion. Then you change out your tool in the machine find and load your offsets to your tool table, go back to fusion at that point with your tools length/dia. and create a single new tool path based on that? It just seems like it would be a lot of back and forth between fusion and linuxcnc. Ive seen a lot of people using just collets in diy routers and thought there was some kind of a work around.
19 Mar 2017 18:54 #89895 by Dougefresh I found this and thought that this is why they were using this configuration. Even if that was the case I still couldn't see how if would all work with the fusion 360 tool table.
20 Mar 2017 08:27 - 20 Mar 2017 08:31 #89932 by Wirewrap
I am doing this in a simple manual workflow.
Typically using three tools, roughing end mill, finshing ball end mill and 45 degree chamfer.
They are modelled as Fusion tools.
All have zero Z offset in LinuxCNC.

1. Design part in fusion, generate toolpaths.
2. Do three POST runs in fusion , one for each tool.
3. Mount first tool, touch off to top of material.
4 Load first tool path into LinuxCNC and run it.
5. Change tool and touch off against a place on the workpiece you know the Z of.
6. Run second tool path

Last edit: 20 Mar 2017 08:31 by Wirewrap. Reason: Spelling and clarification
The following user(s) said Thank You: Dougefresh
21 Mar 2017 13:04 - 21 Mar 2017 13:04 #90002 by andypugh

Dougefresh wrote: Thanks kornphlake, I was thinking that would be the only way... So do you just make multiple copies of your part In fusion and then If you have three tools you would just save three individual files with only one tool path per file?

No, no need for anything so complicated.

In the setup / operation tree in the CAM you can right-click anywhere in the tree and postprocess only that selection.

So, just pretend that you have preset tools, store tool types, diameters, feeds and speeds in Fusion in the normal way.

Then make your post-process selections in such a way that there is only one tool per file. Choose file-names that make it easy to figure out the sequence of ops.

Fusion will automatically put a comment on the top of the file about which tool is used. Read that when you load the file, load that tool, tell linuxCNC that you have done so with a manual M6TnG43 and touch it off to your work or setting plate. (Preferably into the tool table, but either ought to work with this procedure)

Then just run the file.

Practice with birthday candles for tools :-)
Last edit: 21 Mar 2017 13:04 by andypugh.
The following user(s) said Thank You: Dougefresh
22 Mar 2017 00:39 #90039 by Dougefresh
Thanks a lot guys for the info I was having a heck of a time trying to wrap my head around this, I knew there had to be a simpler way!
Moderators: Skullworks
Time to create page: 0.108 seconds
Powered by Kunena Forum