topic Re: Sketch: problem to create profiles inside another profile in Fusion Design, Validate & Document Forum

Sketch: problem to create profiles inside another profile

jmf1DQGCE — Mon, 21 Aug 2017 20:25:33 GMT

Hello,

I recognize that I'm a beginner using Fusion 360. I want to model the wng of a RC glider. The link to the design is http://a360.co/2vTcyQO

Context: the wing consists in 7 airfoil ribs, imported from .DWG in sketches on different planes. Then I loft from rib to rib. I need to include some "spars" in the wing and I try include them in the sketches.

It works well for the first rib T1. The spar reservations appear as independent profiles.

But it doesn't work for T5. The spar reservations can't be selected independantly:

However, from my perspective, I proceeded exactly the same way to create the 2 sketches. I paid attention to snap the vertical lines to the airfoil line... I really need to be able to select the spar profile alone to loft it to T1 one.

I tried to understand what was wrong and looked through the forum without being able to understand. Help would be very welcomed !

Best regards,

JMF

Re: Sketch: problem to create profiles inside another profile

jmf1DQGCE — Mon, 21 Aug 2017 20:40:55 GMT

3 additional pictures to provide information about behaviour:

Re: Sketch: problem to create profiles inside another profile

davebYYPCU — Mon, 21 Aug 2017 22:07:35 GMT

That is weird profile behaviour.

I presume it comes from imported files, Fusion works better with native sketches with my experience.

Away from Fusion a few more days yet, sorry can't read your file.

Re: Sketch: problem to create profiles inside another profile

mavigogun — Mon, 21 Aug 2017 22:58:20 GMT

I reckon you'll have to share the Fusion file- or, at the very least, demonstrate the problem with a screen cast. Is it a selection filtering problem? Does it have something to do with the way the sketches were justified? Have the entire features been rendered unselectable? Pony up the file to some fresh eyes, I say.

Re: Sketch: problem to create profiles inside another profile

etfrench — Mon, 21 Aug 2017 23:05:02 GMT

It looks like the sketch items may not all be on the same plane. Using the 'Move to Sketch Plane' command appears to make it worse. One workaround is to extrude the T5 airfoil section as a component and follow the steps in the solution of this thread: https://forums.autodesk.com/t5/fusion-360-design-validate/unable-to-chamfer-a-created-part-from-a-dxf/m-p/6692858#M82318

When you're finished recreating the profile, make sure the sketch is on the T5 construction plane. You can either redefine the sketch plane or create a new sketch on the T5 plane and project the airfoil section to it.

Note: See Rule#1

Re: Sketch: problem to create profiles inside another profile

jeff_strater — Tue, 22 Aug 2017 03:56:23 GMT

yeah, as @mavigogun says, if we can take a look at the design, we can more than likely figure out what is going on here.

Jeff

Re: Sketch: problem to create profiles inside another profile

jmf1DQGCE — Tue, 22 Aug 2017 05:18:42 GMT

Hi,

Thanks all for your support,

Here are the files. I hope that the format is the suitable one. If not, let me know what I should do.

For me, one sketch = one plane. Can we have objects in different planes in the same sketch ? How can this be checked ?

Last, as my design is in the the Fusion 360 cloud, is there a way to access for you to access to the design in the cloud (read only I imagine) ?

Best regards,

JMF

Re: Sketch: problem to create profiles inside another profile

jmf1DQGCE — Tue, 22 Aug 2017 05:26:13 GMT

@etfrench: your post highlights an error in mine: the airfoil shapes have been imported as dxf (and not dwg).

I have to look in details at your proposed workaround, and reread one more time the Rule #1.

JMF

Re: Sketch: problem to create profiles inside another profile

etfrench — Tue, 22 Aug 2017 06:11:13 GMT

There shouldn't be any difference between a dxf and a dwg import. How was the original dwg created? Was there a reason not to use Fusion 360 to create the original airfoil sections?

Fusion 360 sketches can be 3d sketches. There may be a very small difference in the Z height (90 degrees to the T5 plane) in some of the objects in the T5 sketch.

@jeff_strater, @mavigogun: The file was linked in the first post

Re: Sketch: problem to create profiles inside another profile

jmf1DQGCE — Tue, 22 Aug 2017 07:27:38 GMT

The airfoil shapes are developed by some expert with dedicated tools related to aerodynamics: Xfoil and XFLR5. The standard exchange for those airfoils shapes are .dat ASCII text files with X/Y series. The foil shape shall be precise to 0.1mm.

There is a Fusion 360 plugin to import X/Y/Z csv files, but it needs significant initial .dat file tweaking to get it inside. However there are some small tools to transform airfoil .dat to .dxf (with scaling to right wing size). This worked not too bad up to now even if I have in some cases some difficulties to close the profile.

Thanks for the information about the 3D feature of the Fusion 360 sketches. I have to pay attention to this as it is a bit counter intuitive for basic sketch usage.

JMF

Re: Sketch: problem to create profiles inside another profile

jeff_strater — Tue, 22 Aug 2017 14:27:29 GMT

Thanks. I apologize - I didn't see the link in the original post.

This behavior is definitely interesting. Especially this profile:

I'm not at all sure what is causing this.

However, I know what is wrong. The imported DXF file looks like it has small Z values in it (about 10e-5) or smaller. But, that seems to be enough to throw the profile detection code off. The fix is to select the airfoil geometry and use the "Move to Sketch Plane" command to force everything to be on the plane. Afterward, things behave normally:

One recommendation, however. The DXFs in use here are all made with many small line segments. This results in the highly faceted surfaces that you can see in this image:

You would get better surface quality, and better performance if you re-fit those curves with a native Fusion spline. It's certainly your choice, but might be worth looking into.

Jeff

Re: Sketch: problem to create profiles inside another profile

jmf1DQGCE — Wed, 23 Aug 2017 06:57:16 GMT

Dear Jeff,

Thanks for the analysis and the solution to the problem. I will check tonight on my design.

Complementary question 1:

In order to be able in the future to detect this type of issue, is there a way that I can use to detect in a sketch this type of very small offset ? I had previously done some check by rotating that part of the design, but couldn't see any flaw (my eyes accuracy is worse than 10-5 🙂 ?

Complementary question 2:

Is there a way to automatically transform my many small segments resulting from the DXF import of the very accurate airfoil profile to a native Fusion Spline?

Best regards,

JMF

Re: Sketch: problem to create profiles inside another profile

etfrench — Wed, 23 Aug 2017 07:14:54 GMT

My earlier post shows one way of accurately converting the dxf to native Fusion 360 splines.

If you can't extrude an area, it's a good indication the boundary is not closed or the segments are not all on the sketch plane. You can usually find the non-closed boundary by the divide and conquer method. That is, draw a line splitting the area in two. If one side is closed and the other is not, then the problem lies in the unclosed side. Continue until the problem is isolated. You can also use the extend and trim method to verify all of the segment ends are coincident with another segment end. Using the Coincident operator on the sketch menu may also work. If you can't isolate the problem, then the most likely cause is one or more segments aren't on the same plane.

Unfortunately, Fusion 360 doesn't expose the end point coordinates of sketch geometry so it's not easy to find the errors.

Re: Sketch: problem to create profiles inside another profile

jmf1DQGCE — Wed, 23 Aug 2017 10:49:26 GMT

Thanks etfrench for the tips and explanations.

I'll try all this tonight and will report here.

Merci !

JMF

Re: Sketch: problem to create profiles inside another profile

jmf1DQGCE — Wed, 23 Aug 2017 18:49:09 GMT

So I implemented the "move to sketch plane" function to my airfoil and debug shapes. This solved my sub profiles selection issue. I can also now semlect my spars (the small vertical rectangles. BUT I can't select anymore the airfoil itself (which was possible to select and loft before). By divide an conquer strategy, I isolated the faulty area, but do not see any fault there:

For peace of mind, I reapplied the "move to sketch plane" function" but this didn't changed the things...

Would there be some way forward ? This is interesting for me as I had some similar issues on other profiles that I could not understand. In one case deleteing the sketch and restarting from scratch had allowed getting the thing done, but without being able to understand what was wrong.

In parallel, I study the explanations and workaround proposed by etfrench

Best regards,

JMF

Re: Sketch: problem to create profiles inside another profile

jmf1DQGCE — Wed, 23 Aug 2017 19:20:57 GMT

Humm, I could not extrude (as not closed)...

I made an additional attempt to select the faulty area and apply one more time the "move to sketch plane" function, and it solved the thing... Applying the function to the whole airfloil had not helped.

I suspect some bug here, but I'm not blocked any more.

Will try now to extrude and apply etfrench workflow

JMF

Re: Sketch: problem to create profiles inside another profile

etfrench — Wed, 23 Aug 2017 19:38:03 GMT

I didn't have success with the move to sketch plane routine which is why I suggested the STL export/import workaround. It's clumsy, but does work Here's a screencast to help. I'd recommend doing this to each of the airfoil sections, otherwise the loft will fail. One last thing, I think it would be better to do the entire wing as one loft.

Re: Sketch: problem to create profiles inside another profile

jmf1DQGCE — Wed, 23 Aug 2017 20:13:30 GMT

@etfrench,

I tried your workflow, to extrude the airfoil, then create a mesh from the body, then create a mesh section, then fit curves to the mesh section.

I get my airfloil "profile", it appears in red. but I can't select it to do operations on it like press/pull, loft... nor select sub profiles. Is there something that I don't understand?

Re: Sketch: problem to create profiles inside another profile

jmf1DQGCE — Wed, 23 Aug 2017 20:27:26 GMT

Thank you etfrench,

Your screen cast shows the way ! I now have to learn ! Obviously, Fusion is not really designed/optimized to deal with those airfoils and to transform polylines to splines in sketches.

I recognize that my application is a bit specific.

JMF

Re: Sketch: problem to create profiles inside another profile

jeff_strater — Wed, 23 Aug 2017 21:11:50 GMT

Hi @jmf1DQGCE,

very interesting. There is definitely a bug here in "Move to Sketch Plane", because it seems to take several attempts before all the geometry has been completely moved to the sketch plane. I'm not sure why this is. Here is a screencast showing that, if you are persistent enough, it will eventually all work:

But, this is clearly a bug. I can't think of a reason why the first one should not "take". We will look into that. Thanks for bringing this up. I was so focused on the sub-regions, I did not even realize that the whole airfoil was not recognized

Jeff