Creating a celtic knot

[Arcathorn]

Morning everyone,

I am looking for the best method of creating a celtic knot in fusion 360. I have a design in mind and have done some experimenting but I have to be honest my results have been mixed. When I have done it in the past in inventor I have used a series of sweep commands but for the most part the results are pretty clunky to manipulate. One of the reasons I have been so excited for this new software is its ability to manipulate bodies without being constrained as much as inventor is. However after some extensive trial and error I have not found an efficient way of creating this design. I am attaching an image for you to reference and I would appreciate any suggestions that you could give me.

[Arcathorn]

OK as an update...I was able to get a pretty good result using a tspline body sweep. It gave me the look I wanted however what I am confused about is this...sometimes after the sweep the body would change from smooth to boxy. I am assuming its because it doesn't have enough faces or edges to maintain the smooth look I wanted. I started trying to find some way of changing the body to include more edges or face just by clicking on it and getting that same dialog box that came up when I initially created it but I couldn't find any such controls. Do you have to go in and manually add more edges to each section of the body? It would seem that would be a big job giving the complexity of the model. Oh...and it crashed so I lost my work because I didn't realize you have to click save to have it update...that and I got on a roll...but isn't that always the way. Well still looking for tips and suggestions on this idea of mine.

[Mike.Zhang]

Just give you some tips, you can use the 3D sketch in Fusion 360 to create it, then use the Pipe command to create it.

You can invoke the 3D Sketching in Preference, showed in below image. Hope it'll be helpfule to your design.

Another tips, you can use insert image button to insert your image into the comments, so others could directly see it, don't need to click it one more time.

[Mike.Zhang]

[Mike.Zhang]

[Mike.Zhang]

Attached one more better celtic knot image for your reference, hope you can succesfully make it.

[Anonymous]

Hi Mike that is one of the best 3D sketching illustration I had seen so far! Thanks for doing that!

[Arcathorn]

Wow. Thanks for all the really great tips. I didn't know about the 3D sketch command. That will make the job a bit easier. However I am still curious why it changed from smooth to boxy at times?

[Arcathorn]

So I worked and worked today on this model. I manipulated the body to get exactly what I wanted. Some of the knot lengths interest one another to create a stronger point for 3D printing...however when I went to convert it to a solid it errored and said it was self interseting. So is there no way to convert this to a solid so I can export it to an STL?

[Anonymous]

Hi, if you used the "Pipe" command at the "Model" workspace to create this design, it is already a solid. If you felt that you could use the "Convert" command at the "Sculpt" workspace and got a response you might have a mixture of "solid" and "T-Splint" bodies in your design. Usually if a design is already a solid you will not see any "highlights" when you are moving the cursor around the bodies. So I do suspect that you have a mixture of both or you had made the design with the "Loft" command in the "Sculpt" workspace. Then you will see some highlighting when moving the cursor over the bodies. That is when a T-Splint is already converted into a BRep or "solid" "Convert" will not generate any result.  Go to Box mode and take a look. Converting T-Splints to Solids  you do have to correct intersecting faces and edges and the way it looks in your screen shot you do have some intersection. If it is still a T-Splint, try raising or lowering the intersecting parts to prevent the intersection then you might be able to convert.

One way to test my "mixture of T-Splint and Brep bodies" theory is to select "Command" at the "Sculpt" workspace and kind of moving the cursor around the design and if you saw some highlighting on some parts of the design and not all of it, then the theory is correct.

That is only my own experience.  Mike or other experts in Autodesk can give you better solutions and possibly can share with you and correct that for you. But I would like to share my experience with you too. This testing theory might help your future designing with Fusion360.

Well Merry Christmas! And I hope you got what you wanted. It is a long road to learn using any 3D program but you will find new tricks every minute and it will burn into your mind and you will feel great using them eventually! This Community Forum is a great way to learn!

From you designer friend from Asia.

[Anonymous]

Let me give you one example of carefully moving parts to prevent intersection. This is a screen shot of a Pendant design called "Network" and lots of time were spent to put the parts together so they do not touch each other. This pendant will move with the wind and any slight body movement. Always go back to the original shape. One of my most favorite design so far! Once you moved the parts and converted successfully into Solid, then you can move them back together to form strong points. But beware of STL file error.

[Arcathorn]

Wow that pendant is pretty hot.

And no the body is not a mixed one. I used all tsplines to create the part.....trying to get the wires to not actually touch might be a bit hard and cause some undesirable deformation. I will take another crack at it tonight. I didn't think that this would be an issue and I can think of a few ways I might be able to get around the problems but it will require some trial and error....I wonder if I can combine the bodies into one giant tspline and then it wouldn't care about self intersection...hmm I will have to try it out. I will let you know what my results are

[Anonymous]

Since I noted that you actually used a few TSplines to form this design. You can convert individual TSlpines one by one then combine them together. You can make some TSplines invisible by clicking on the light bulbs of the TSpline bodies then convert the ones still lighted. Do that one by one. You will see the solids formed in the Body section of the Browser. Then it might work. I actually tried this before because I had the same problem when converting different TSplines at the same time. Sorry i edited this reply a few times because I wanted to test the theory first. I think this one will work.

[deyop]

Unfortunately neither solids nor T-Splines will allow self intersection during construction or conversion.  This is the case with solid as well if the sweep path creates a body that self intersects.  Kingson's advice is sound and for now we would have to create separate solid bodies that could be subsequently intersected.  Here is an example shown with two diameters one that self intersects and one that doesn't.

There is another problem of when a single T-Spline body has self intersecting faces.  This is a bit different and can happen when the body is less complex than the Celtic knot you are working on.   The smooth mode is deceptive in that you aren't seeing the underlying control structure that represents the math behind the surface.  The Smooth Mode may not appear to self intersect but if the box or control frame do intersect than conversion will fail.  To find the self intersection it will help to have the model displayed in Box mode.  There is a command for this under Sculpt - Modify - Display Mode.  However since since seeing the structure is so important to downstream conversion operations as well as improved performance you can always switch models between different display modes by having the model or any portion of it selected and using the Alt (Windows)/CTRL (Mac) - 1(Box), Alt (Windows)/CTRL (Mac) - 2 (Control Frame and smooth model) or Alt (Windows)/CTRL (Mac) - 3 (Smooth).

When you are in Box display mode look for those nasty intersections.  Manipulate the vertices, edges or face in Edit Form to untangle the T-Spline.

We have developed a way to show the location of intersections and will be releasing that in the future but for right now you have to search for the problem areas.  The place to find them is generally in areas where there is a high concentration of edges.

Sorry for the trouble.  Hope you can get a successful conversion.

[Arcathorn]

Thanks for the tips!! This community is awesome for feedback.

I practiced a little last night at trying to bend the parts up but I think I will go back to the beginning on this....Where my mistake came was the intial build. I sweeped the tspline and then mirrored the original to get my shape. Then I went in and bent the lines to get the look I wanted....I think what I will do this time is sweep....create a seperate body...mirror a new body.....then mold it to the shape I want....seperate them...convert...and then put them back together and combine. That should solve the issue and give me the look I want without causing fusion to have a heart attack..

With the 3D printing process the self intersection is a must to give certain joints additional strength. If they don't meet the joint will look good but it will be weak. I think this method is the way to go....and next time I do something like this I will know exactly how to do it and can cut my design time down to a couple hours instead of days...

I remember the first time I tried to do it with inventor..............oh my god was that a nightmare. Talk about constraint errors 😞 I do love this new software but coming from the mechanical world the organic modeling process is very different then what im used to. The moment I am successful I will post a screenshot and a link to my shapeways page........just in case any of you are looking for a late christmas gift ; )

[Anonymous]

Hi you do not have to separate them, try the light bulb technique. Then light them one by one, and then light off.. after that you have a group of solids formed. light them all up and combine or form components. Hope for the best! Yes we would like very much to have your Christmas Gift!

[Mike.Zhang]

Hi Kingson,

Thanks your comments, your replies are very good.

Hi Arcathorn,

Hopy you can successfully solve it.

Merry Christmas to everyone ~_~

Regards,

[Anonymous]

Hi Everyone here, Merry Christmas!

[Arcathorn]

Still have not had the oppurtunity to get back to this design. But I wanted to wish everyone a happy holiday

[deyop]

Happy New Year to you.  We are doing some experimenting with the intersection conversion and may have a solution to share with you shortly.  I will keep you informed.