Inlays for Wood Letters and/or Designs - F3D Attached

[mcarpenter28]

Good day all - I have seen several postings regarding Inlays, however nothing that addresses the multiple designs I am working with.  Specifically I was following a post on a guitar fret-board, however the inlays are straight and flat, which is not efficient for shapes and text. Below is a link to a similar process from Broinwood, who uses a "v carve" method, which leaves a tapered and smaller edge towards the top, and a larger base that is cut off and fills in the void/pocket cut out - which is also done with a v-bit.

While I have attached these F3D files, I am trying to avoid using VCarve or Vectric software for this process. I am a huge Fusion 360 fan, however this process is not intuitive at all nor can I find any tutorials to figure out how to best create to files, one with a male and one with a female component, which will fit together and leave zero gaps. 

I have tried multiple cutting methods, from trace, to Engrave.  Engrave seems to work somewhat, but requires a guessing method to ensure the parts align.  Perhaps there is a way to "fit" the components together through the assembly option in Fusion?  Willing to try any method or provide different files.  Just looking for a way to make this work as I have a ton of different inlays I want to accomplish, and need a quick and efficient way post drawing to make this happen.

Link to Broinwood Samurai Star Inlay

[g-andresen]

Hi,

Take  a look at some of these tutorials

günther

[mcarpenter28]

Thank you, I will review today and reply.

[g-andresen]

Hi,

Here is a basic tutorial creating v-carved inlays.

Günther

[mcarpenter28]

@Anonymous, as a rated “mentor” I am very surprised at your reply. I blocked off an hour to dive into your response, only to realize you performed an inlay search on YouTube. Perhaps my extremely documented question wasn’t clear enough to obtain that the videos posted do not discuss literally any detail needed to make this work. I appreciate your in-depth knowledge and time spent on using a search engine. 

If anyone has in depth knowledge of vCarve inlays, please let me know.  

[g-andresen]

Hi,

I would like to clarify that I am referring to sources here, some of which I have used myself to gain basic knowledge for creating inlays.
I have been able to successfully complete several projects based on some tutorials, but I don't see the point of repeating their contents in my own words.
Also, despite several years of experience with Fusion, I would still use V-Carve for inlays.

günther

[djlunty]

@mcarpenter28 

As you have discovered Inlays in Fusion 360 are not straight forward.  If you do a search on the forums for V-Carve Inlays you  will find some posts that discuss the subject and different methods are illustrated.  Also check out this link from another forum

https://forum.onefinitycnc.com/t/recipe-for-creating-v-carve-inlays-in-fusion-360/1989

I am in the process of documenting a method I am working on.  Attached are a PDF of the documetation and a .FD3 file that I am experimenting with.  I do a bit of extra work on the design workspace just to keep things organized.   I find it easier to work with models rather than just sketches. The goal was to use the V-Bit to create the edges of the inlay and pocket and use flat endmills to clean out what the V-Bit left.   Not sure it works in all cases and with diffetent V-Bits, Ratios and Depth of Cut.  More testing needed.  If I get a chance tomorrow I will see if it works with your files.   Good Luck!

A comment regarding the method Broinwood uses is at the following link 

https://forums.autodesk.com/t5/fusion-360-manufacture/sharp-interior-corners-with-a-tapered-ball-nos...

Doug

[TrippyLighting]

---

@g-andresen wrote:

...
I have been able to successfully complete several projects based on some tutorials, but I don't see the point of repeating their contents in my own words.
...

---

I can see that point, but to a degree I have to disagree .. to a degree 😉

What happens cognitively when reading documentation, watching different tutorials for different software and observing different workflows, is that slowly but surely we start "connecting the dots". That is something that happens gradually and perhaps not consciously.
A user that watches a small selection of the same tutorials we have watched over possibly much shorter period of a time might not experience the same effect.

As such a good explanation often helps that process.

[mcarpenter28]

Thank you DJLUNTY - I have watched so many videos and read stacks of documentation that I am finding the same.  I appreciate you documenting this, as I may do the same based on what have found out, and what I have yet to find.  The straight boxed out inlays are what most people focus on, while the intricate and fine detail inlays are what people want.  I am not convinced that a "v carve" is the solution, as I found a video on the slope of an angle matching the slope of a tapered end mill bit can reduce some of the errors, its just frustrating that a program as complex as Fusion and with the unbelievable talent they have and in this forum, that there is not an add in for 360 or tutorial given the popularity of this method.

Thanks again!

[mcarpenter28]

I would even settle for a simple rectangle or letter, with both the pocket and inlay provided in F3D format, just so I can see the manufacturing process selected and could play with the settings for some more trial and error.

[TrippyLighting]

I am going to tag one of our CAM experts to chime in or summon reinforcements @seth.madore 

[seth.madore]

I've not personally done any inlay work in Fusion, full disclosure. I do know that there are benefits to using software that's actually designed to do this, rather than hacking something together in Fusion. That said, I will point you towards this informative thread where a good discussion took place:
https://forums.autodesk.com/t5/fusion-360-manufacture/v-carve-inlay-anyone/m-p/6583570#M17489
https://forum.v1engineering.com/t/vcarve-inlay-technique-with-fusion-360/14415/51

I realize that both of these are not a direct answer, but it's what I've bookmarked since the last time this question was raised on the forums

[djlunty · Accepted solution]

@mcarpenter28 Here are files that I created.   Started with just your sketch - deleted the rest of the model. Combined the heart with the remainder of the pocket component - you had it split.  Have not run on CNC but looks okay in simulation.  I used the following initial parameters - DOC = 0.200 inches, R = 0.667 and VBTA = 60 deg.  In the Pocket Setup the first two tool paths are supressed - pocket is too small for them to get into.  The third tool path with the 1/8 inch tool does  not machine all the pockets as some are too small.  I used my tool library as as I plan on running this on my CNC.  I think I kept all the other settings that are in the previously attached PDF except for

Inlay 3D Adaptive - Radial Stock to Leave changed to 0.1

Inlay 3D Pocket - Radial Stock to Leave changed to 0.038

If you get tool paths that don't generate try adjusting the Ramp to Plunge.

If you get goofy tool paths with REST Machining try changing the Adjsutment Offset - this link gives a good explanation of the Adjustment Offset

https://forums.autodesk.com/t5/fusion-360-manufacture/3d-adaptive-and-3d-pocket-and-rest-not-playing...

Also saved the stock after simulation and inserted into a new file (heartbeat mesh.fd3).  Used Rigid Joint to combine them and did some section analysis.  You can Edit the Rigid Joint to move the Inlay (the top component) to see how it all fits together.  Created a sketch from the third section analysis and added some dimensions. Show the space left for glue and the gap needed to cut the pieces apart.

If something does not make sense just ask.  I will try to answer but I am figuring this out as I go ----------

Doug

[mcarpenter28]

Very helpful and I appreciate all the work done here.  I have downloaded the files and will play around with the setting son my CNC machine.  In the interim I downloaded VCarve Pro and Desktop versions.  They have automated this process but I have been in Fusion for so long I cannot bring myself to but the software as I am used to 360 but enjoy the flexibility.  I just wish someone could reverse engineer what VCarve has done with their V Carve process for inlays. 

Thanks Again.