Engraving Text with Fusion 360

[dbeetcher]

I've been trying to use Fusion 360 to engrave a simple line of text on a flat surface. Unfortunately I can't seem to figure it out! I have tried numerous examples I've found on the internet (F360 forum, YouTube videos/tutorials, etc.), but when it comes time to select the contour of the text for engraving, it won't 'select' properly. Then when I try to generate the toolpath, it gives me an error message:" Warning: No passes to link. Error: Internal CAM kernel error. Please report through your support channel."

Could anyone give me a step-by-step set of instructions that I could follow (to the letter) so that I could get this to work?

If it would help in troubleshooting my problem, I could put together my own set of instructions and screen captures to explain exactly how I've been trying to do it (unsuccessfully).

By the way, I uploaded the latest version of F360 yesterday.

[dbeetcher · Accepted solution]

Update to my previous post:

Through very, very careful execution of my own instruction steps, I was finally able to successfully make sketches and a model to engrave or trace a single line of text on a block using only the Engrave/Trace features of F360. I was also able to build and execute a simulation. So that part of my problem seems to be figured out, or at least I found a work-around. But the next step would be to generate G-Code for my Mach 3 CNC system, and now I'm having problems there.

Tonight I will see if I can successfully post-process on a simple block-squaring job with errors. Not sure if this version of F360 is causing me problems or not, just got it yesterday and this is my first attempt at using this version.

Here is the error log file I got during the post-processing attempt, maybe someone can spot a simple error:

Information: Configuration: Generic Mach3Mill
Information: Vendor: Artsoft
Information: Posting intermediate data to 'C:\Users\212008774\Desktop\CNC\G-Code Files\1002 Fillet.tap'
Information: Total number of warnings: 1
Error: Failed to post process. See below for details.
...
Code page changed to '1252  (ANSI - Latin I)'
Start time: Monday, June 06, 2016 6:08:45 PM
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.2.1 40504
Configuration path: C:\Users\212008774\AppData\Local\Autodesk\webdeploy\production\13fa4f7ba18b18f6fd68cb6ab44ba992e0a1b19e\Applications\CAM360\Data\Posts\mach3mill.cps
Include paths: C:\Users\212008774\AppData\Local\Autodesk\webdeploy\production\13fa4f7ba18b18f6fd68cb6ab44ba992e0a1b19e\Applications\CAM360\Data\Posts
Configuration modification date: Tuesday, February 09, 2016 2:30:23 AM
Output path: C:\Users\212008774\Desktop\CNC\G-Code Files\1002 Fillet.tap
Checksum of intermediate NC data: 773e148c60273b5c6281e5948834665e
Checksum of configuration: 7b530218354d96dac5560b776c43cd70
Vendor url: http://www.machsupport.com
Legal: Copyright (C) 2012-2016 by Autodesk, Inc.
Post processor signature could not be verified (error 0xfffffffc).
Generated by: Fusion 360 CAM 2.0.2087
...
Warning: Work offset has not been specified. Using G54 as WCS.
Error: Tool orientation is not supported.
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
Error: Failed to invoke function 'onSection'.
Error: Failed to invoke 'onSection' in the post configuration.
Error: Failed to execute configuration.
Stop time: Monday, June 06, 2016 6:08:45 PM
Post processing failed.

[Stuart-H · Accepted solution]

Hi

try turning off set tool orientation off

you have a standard post that does not have it tuned on 

been there done that got the tee shirt

Stuart

[jeff.walters]

Warning: Work offset has not been specified. Using G54 as WCS.
Error: Tool orientation is not supported.

This is saying that your Z orientation in your setup is incorrect to the tool paths (and probable the reason you have been having issues to start with). In order to tell you more I would have to see your part. Can you export it as an .f3d and post it here?

[HughesTooling · Accepted solution]

If you only have a 3 axis machine Tool Orientation in an op should not be activated, you set the origin and orientation in the setup only.

In an op leave tool orientation unselected.

If you have 4 or 5 axis you need a post setup for it and your machine.

Mark

[dbeetcher]

Hi Stuart,

Thanks for your suggestion, that was the problem. I was incorrectly using that tool orientation button to change the orientation of my XYZ axis. Apparently F360 defaults to having the Y axis as the vertical axis. I went into Preferences and changed the General > Default modeling orientation setting to 'Z up' and everything is fine now. Thanks to everyone else that directed me towards the right solution!

[Anonymous]

Can you share your step-by-step instructions?  I've been having the same problem.  Sometimes when I add text it put it in upside down and backwards.  WTF   Can't believe engraving letters could be so complicated.  Very frustrated.

[tugs]

Will someone please post a step by step instruction on how to engrave a simple few letters of text via Mach3. This has to be the most frustrating exercise possible!

How do I generate a toolpath? What magic is involved in selecting the text to be processed into code?

Will someone at Autodesk please make a video devoted to  drawing a flat plate with a row of text then generating the G code for Mach3 so it can be engraved.

[ivan.stanojevic]

@tugs

I recommend you to watch these couple of videos:

https://www.youtube.com/watch?v=cNgk46XRMVg

https://www.youtube.com/watch?v=hQbz8abi3RU

https://www.youtube.com/watch?v=TMVxzPZeRls

https://www.youtube.com/watch?v=aUbWAdIXUqk

[dbeetcher]

Hi Tugs, I've been working on the steps needed to engrave text using Fusion 360 as the CAD/CAM software and Mach3 as the CNC software. If you still need some help (after viewing the YouTube videos that Ivan suggested) I'd be glad to share my recently-acquired knowledge!

[dbeetcher]

Hi mkbrummett58, do you still need some step-by-step instructions? Sorry, but I didn't see your request from back in January. So if you still need some help, let me know.

[Anonymous]

Do you still have the steps written out? I would LOVE to have them.

I am 100% new to Fusion 360 and only started learning it in order to learn to engrave aluminum. I've watched hours and hours of videos, tried Easel first, then Fusion 360, then Inkscape. I'm computer literate, have programmed in several old school computer languages, and  I have used graphic software. This engraving task has me stumped!!!

I am trying to engrave single line text,  with 3mm tall letters (I found the correct single line fonts to use).

It's been extremely frustrating

[johnswetz1982]

@Anonymous  If you are trying to use the [Engrave] operation for single line font it will not work. Try a [Trace] operation for that. Engrave is meant for double line text where the tool path pulls up vertically in corners so that sharp corners are maintained.

Even better if you can go File>Export>*.f3d and attach your project here someone would be able to show you an example of what you need for your project.

[HughesTooling]

Machining into harder materials you might want to try 2d Contour for single line fonts and set the compensation to off so you can ramp down rather than plunge using Trace.

@seth.madore  I noticed with Trace or Contour the toolpath is offset from the text. If you explode the text to curves it's correct, so something odd machining direct from fusion's text. Sample file attached. Different fonts seem to give different offsets.

Mark

[seth.madore]

I've opened up CAM-26572 to investigate this issue, thanks for the report @HughesTooling