Image relief, any way to create one in Fusion360?

[Anonymous]

Is ther a way to create an image relief in fusion360 from a black and white image? I'm thinking of something like imagecarve or vectric aspire.

I'm asking because there are some very clever people  here and someone may have a workaround or something that I missing.

[innovatenate]

You might check out Inkscape. It will convert raster images to vector. Once you have a vector format (SVG or DWG), import into Fusion 360 and then you can extrude to cut out material. 

Something like this may help!

https://inkscape.org/en/doc/tracing/tutorial-tracing.html

Thanks,

[HughesTooling]

There's a program called ZSurf that converts bitmap images to 3D NURBS surfaces in IGES format. I'm not sure where best to download from, after a search I found this link.

Mark

[Anonymous]

Zsurf works awesome !

I can convert images to a "skin" very easily. What I have trouble with now is using that with a Fusion360 model I already have.

For instance, I sculpted a wooden tray in fusion360 and have actually machined 2 of them as gifts.But I would like to add a Celtic swirl to the face of the serving tray. I now have the swirl from Zsurf converted to a .igs file.

I created a new model of the swirl in fusion360 from the igs file and now I dont know how to incorporate that into my existing tray model.

I don't even know the words to use to search for a solution. lol.

Any guidance would be appreciated.

I included a link to the file if anyone is so inclined to try to incorporate the swirl and post a solution. That would be such a great help!

thanks

http://a360.co/1PLNLkj

[sebmorales]

What you can do is create a simple square the size of the drawing and then extrude it to the surface you imported, then you would have it as a solid body that you can join to the try. I recorded a quick video showing the workflow. 

Hope this helps!

[Oceanconcepts]

There are multiple ways to do this. You want to get to a solid with this as a face, positive or negative depending on your intent. This kind of imported shape is very complex and irregular, as compared to what you would get if you modeled it inside Fusion, and operations like thicken will probably fail. 

One other method is to use the surface as a splitting tool to create either a positive or negative solid version of the shape to then use to either subtract from your tray or add to it in a boolean operation. That’s what I show in the screencast. 

I did extend the sides a bit-.05”- in the patch workspace, as it looked as if part of the shape was cut off. 

I also moved the patch surface to align with the origin plane, making creating a box to align with it a bit easier. But basically just making a box, then using the surface to split it. This will give you two solids you can use on the tray.

[Anonymous]

@sebastian

Thank you for your solution, I'm trying to implement it on a more complex project.

[Anonymous]

@Oceanconcepts

Thank you for your solution.
I've been trying to work with this method. It makes perfect sense, but I have trouble locating it directly on the surface of the tray for a combine cut. It seems that the depth and placement is merely trial and error.
If you have a suggestion as to accurately placing the the one half on the tray for a combine procedure - I would greatly appreciate it!

[Anonymous]

Btw, this is what I have so far...!

[Oceanconcepts]

re. positioning, you have a complex shape with no obvious points or planar faces to snap to, so it may well be trial and error. But if you want to be more precise in the vertical direction, you could

1) make a sketch within each component perpendicular to the surface at the midline (activate the component first, so the sketch is inside it in the browser), then

2) use the Project-Include- Intersect tool in the sketch menu to create a cross section as a sketch curve. You could then

3) create a line or point in the sketch where you want the surface to mate.

Do this in both the tray and the cutting tool, then use the Move or align tool (move/ align components option) to snap the two components into alignment using the sketch elements as alignment points.

You may want to create a construction plane on which to base the sketches first, if the origin is not positioned in the center of the components. If you want to get really precise, you could create top view sketches, project the outlines of the components, then find mid points for each to precisely center in the horizontal direction. Basically use sketches within the components to provide references for moves.

[donsmac]

The resulting model from zSurf does not have a edge that is planar so it cannot be lined up with the planar surface of the tray. 

The image you used to create the zSurf model was of low resolution to start with so the model's surface is relatively rough because of that. 

To get a better zSurf model add another circle to the image before you send it to zSurf. The idea is to get a flat surface inside the outer ring. Afterwards cut the outer ring off resulting in a planar edge: 

I have not tried this but it makes sense that it would work.

[Anonymous]

You are absolutely correct.

The image I used was not setup correctly for a useable result from zsurf.

Thank you for the workaround.

[Anonymous]

@Oceanconcepts

I am very interested in accuracy of placement.

I worked with you suggestion, and have it worked out all the way to snapping the component in place using the sketch entities.

This is where Fusion360 falls apart.

- OR -

I'm missing an important step in moving a component. But, the component (I'll call it a Die) of the swirl , when moved , has no reaction between the sketch entities within. It is impossible to locate the "MOVE" pivot point to a specific point on the component for that matter. So Fusion seems very "not for prime time" regarding moving components accurately.

Would joints be more applicable in this application?

BTW: Im really impressed with the split body approach you suggested earlier. That has uses for me that are endless - thanks

[donsmac]

I've done a screencast of how to do this within Fusion, it's about 18 minutes long but I included a bit of trouble shooting:

[Oceanconcepts]

I made a quick and rough screencast showing some options for precise alignment. I’m not sure if you are missing some of the tool options such as controlling the manipulator and pivot points, hopefully this will help. 

There are many ways to do things in Fusion, joints would be one, but since the goal is to use the body as a cutting tool that seems an odd use to me. I can’t think of any reason it would not work, but it would leave a joint object in the browser. You could edit the joint there, so maybe that would be a good thing. The method that comes to me involves setting up a parameter to control the depth of cut. 

Align and Move tools will both do what you want. The only issue here is that the shapes of both the knot pattern and the tray are irregular, so we need to make sketches in the components to provide a handle for precision manipulation. 

[Anonymous]

Brilliant!

thank you for explaining the use of the sketches, and point to point snapping to locate the parts.

yes there are several ways to accomplish this  task and I drew on all suggestions in this thread so far.

I worked it out using joints and joint orgin location on the tray, and also a projected sketch from above to locat x & y location for a joint.

Your solution involving a parameter connected to the z depth is brilliant! I am going to try this method.

here is another application with the same tray but a little more complex image..

I only wish Fusion360 could process images within like ZSurf can... it would be so useful.