Variable radius fillets

[NorthHighlander101]

I'm a noob regarding Github, so please forgive if this is not appropriate.
I've recently taken up Layerling following high praise of it on various YouTube channels. I agree. The praise is well justified.
I am a long term TurboCad user, only on the Deluxe version and, so far, it has done me well.
However, in the hobby work I put it to, there are deficiencies.
Layerling has addressed all these deficiencies... except one (so far!)

I have an object with one straight face (i.e. perpendicular to the base) and a slanted face at around 80 degrees to the straight face. I want to be able to apply a taper chamfer which respects the straight face but increases in radius as it moves down the slanted face.
Is such a feature within the possible capability of Layerling?

[henmedia]

@NorthHighlander101 Your question fits here perfectly. layerling can do it now, out with 1.98.0: in the fillet window switch on "Variable radius", pick the one edge, and set "Radius at the start" and "Radius at the end". The radius grows evenly along the edge; "Swap ends" puts the larger one at the other end. It works on one edge at a time.

If you'd like to support the project, a small donation is very welcome. 🙂

[henmedia]

@NorthHighlander101 thank you for the file, it let me test it. And yes, I answer fast, but I am sure you are not the only one asking. 🙂

The cause is not the variable radius: even an even fillet fails on that corner. Your part is an imported STL, and its curved bottom is made of seven narrow flat strips, each less than a millimetre wide. The corner runs into those strips, and a radius of 1 to 2 mm has no room there. A very small radius, a few tenths of a millimetre, still works on it.

Since you work in TurboCad: export the part as STEP instead of STL. A STEP keeps the bottom as a true curve, and then the fillet has a smooth surface to run into.

[henmedia]

@NorthHighlander101 thank you for the file, it showed me what happens. I opened it and tried the fillet on single edges. It works at 0.1 mm on the top edges and at 0.5 mm on some of the long edges, but a bigger radius fails with "cannot be filleted at this size". The reason is the model itself: next to those edges there are very narrow faces (0.22 mm at the top, about 0.5 to 0.6 mm elsewhere), and the curved lower edge is cut into six small pieces of about 3.7 degrees each. A fillet cannot be wider than the face beside it.

Two ways that should help: build the corner post in layerling with a sketch of its profile (the curved edge as one smooth curve, not as many small faces) and extrude it, then fillet the long edges; or fillet the corner before the small details are added to the model.

How large should the rounding be at the top and at the bottom, in mm? Then I can try the same corner on my side and tell you what works.

[NorthHighlander101]

Thanks for the (as usual) speedy reply, Stephan.... I will get some brain restoration now (aka sleep) and work out the various dimensions tomorrow. It might take some time. Meanwhile, another idea post will be forthcoming..... TurboCad deLuxe does not export to STEP. For that I would need to purchase the Platinum version which would cost me approaching the UK's annual GDP I think. I think that I actually created the object in the file I sent in Layerling by creating a box to which I then added a sketch of the curved profile and extruded that as a hole which combined with the box resulted in the object. However, I wouldn't swear to that, as I earlier used a test piece created in TCad and saved as STL hich I then imported to Freecad (who?) to convert to STEP. That was a tortuous process..... the Idea I will submit is to have a <filetype, including STL> to STEP converter in Layerling...

[NorthHighlander101]

Good morning from a windy and wet Scotland!
The weather is a good excuse to stay indoors and complete the action I promised on Friday.
I have attached two jpg files of the corner post, one the wireframe and the other the solid of the same model. I hope that the dimensions including the three radii are clear.
For my hobby I always draw full size, normally in inches imperial, which can then be scaled in the slicer. (for some reason, which I cannot understand, is that Bambu slicer takes the STL file and assumes that the numerical dimensions, drawn in inches, are millimetres. I'm not complaining because it's then a simple matter to rescale to 33.33% to get to my required scale of 1:76.2!)
The model is is two parts, the upper part has a straight face on both sides but the front is angled back 2.47 degrees to the perpendicular. The lower part has one face (the tumblehome) radiused to a non-constant radius.
In plan, the left hand face is shown in the images is angled 8.94 degrees from the rest of the model. The rear and right hand faces are at 90 degrees to each other and perpendicular to the base.
If you have any questions (I am sure that my amateurish attempts at drawing might be confusing) do please ask.
I tried to save the model as an .stl file and import to Layerling but it announced that the model had over 6,000 triangles! I am not experienced enough to understand how to successfully convert stl to STEP.
Surely, if you can solve this (what seems to me to be) impossible variable radius model, Layerling will be able to solve ANYTHING!
Many thanks though, for all your help and advice.
Meanwhile, back to storm Boelo.....

[NorthHighlander101]

For information. this is the sort of corner I am trying to reproduce......

(Copyright SR Official copied from cover of 'Southern Electric' by David Brown publ Capital Transport)