Still feel lost with 3D Sketching in Fusion

[cekuhnen]

I understand why the sketch engine in Fusion works differently like in Alias or Rhino.

And while I miss curbe tools such as blend curves etc I see the point.

However I really do not get along with the 3D sketch engine. I find it very cumbersom to use

and very unproductive.

First the snapping does not work when the sketch is not on the sketch plane.

Whats then the point of 3d sketch when I cannot snap? And this with-in a sketch.

Snapping also thus does not work when I try to make a sketch the snaps to two other sketches.

Second you calso cannot rotate a sketch element you can only move it along x y z or you rotate the complet sketch at once.

Now my question is if maybe I misunderstand what 3D sketch should be in Fusion or how to use it properly.

What is the targeted intent for this tool?

[innovatenate]

I suspect you may need to use the project sketch tools and sketch constraint tools more. The project sketch tool build a reference between external geometry and internal sketch figures. Look for these command in the Project/Include fly out menu of the Sketch drop down.

These can be powerful when updating models in since sketch figures will update based upon 3D geometry. Projected geometry in Fusion 360 is a different color (e.g. magenta in the Photo Booth Environment setting). You'll note that if you right click on projected geometry, the "Break Link" command will be available.

The next step is to build relationships to this projected geometry. For me, snapping is great for quick placement of sketch figure; however, the snap doesn't create a relationship between sketch figures in a really meaningful manner that can update as geometry updates. In Fusion 360, sketch constraints are the mechanism that will create a relationship between sketch figures. These usually should be done in a methodical and predictable manner for the best results.

I made quick video below that shows the work flow you may use to connect 3D sketches with other sketches. I hope it helps. 

Please let me know if you have any further questions or feedback. 

Cheers,

[cekuhnen]

Thank you for the pointer and direction - pretty labor intensive work for just even basic shapes already.

Here are some observation and suggestions.

In my video I start with the same thing having to flat sketches.

The first thing that highly annoyed me was that to be able to make the sketch constraint

to the geometry inputs I needed to 3D move the sketch once. This should not be required.

https://drive.google.com/file/d/0Byzv_NlyKp_2eTBTbEZxLWVlQ1U/edit?usp=sharing

Secondly to be able to use the edge constraing I need to define the point constraing first.

The software like in others should be smart enough to understand which end of the edge

should be constrained to what end of the target edge.

And when I add a point to the spline and move it the edge constraing also gets overwritten

so I have to add it again - while it is still there but not working.

https://drive.google.com/file/d/0Byzv_NlyKp_2Y0Rfa19XelR0Zkk/edit?usp=sharing

Besides constraints which seem to really have their use - I feel good snap is still a tool

Fusion lacks and thus also for me makes product placement very inefficient.

For example I cannot just align a point along x and y in reference to the point on the

spline below. In Alias or Rhino this would be easy.

https://drive.google.com/file/d/0Byzv_NlyKp_2b2FSZkotTTdQWlU/edit?usp=sharing

I also seem to be able to make the edge just snap to the points of the spline and not

the spline point snap to the edge points. INterestingly in the video the tangent constraint

of the spline remains intact while the point got pulled to the line. Deleting the line actually

also does not make the spline mid point snap back where it was.

https://drive.google.com/file/d/0Byzv_NlyKp_2d3kxZjRVZHFaMEE/edit?usp=sharing

I was also unable even when I add another sketch and again inlcude edges / points from other sketches

to make the line perpenticular to a line or such.

https://drive.google.com/file/d/0Byzv_NlyKp_2Y3BpS3d6c08xVjA/edit?usp=sharing

Again this drawing would be a snap in Rhino with the drawing / snap tools it has.

I feel while the constraints have a real value because you work with dimensions they

are also quite restrictive in the way how fluid you can work and what you even can do in Fusion

in it's current state.

If you have any insight I would highly appreciate it.

[cekuhnen]

How when I tangent constraint the curve can I adjust the flow of the spline curvature and how quickly or smoothly it flows into the target edge?

[cekuhnen]

Here is a quick screencast of the problem I see when you work with the spline point handles to adjust the curvature.

https://drive.google.com/file/d/0Byzv_NlyKp_2WGdXTUQ4T0xTUDg/edit?usp=sharing

The tangent constraint ignores the handles or does not line them up and when adjusting again the constraint gets over written.

[cekuhnen]

Here in my last video I tried to have a third spline inbetween for a Rail which does not exist (yet?) in Fusion. I have no idea if it is possible to add the center spline and make it constraing to mid points of each edge and then make it perpendicular to the edge and tangent so it flows into the surface.

https://drive.google.com/file/d/0Byzv_NlyKp_2QkFLRENEMWc2ZlU/edit?usp=sharing

SolidThinking will allow me to do with with their parametric design tree. Or is this a step which is not ideal for solid modelers?

[innovatenate]

Claas,

This is awesome feedback, thank you!

There definitely seems to be an issue with the Tangent constraints disappearing when you move a control point on a spline. To my best knowledge, that shouldn't happen. However, I will have to forward this to development for further investigation. I know the below video doesn't address all of the issues raised above, but it does show that you do not need to use the move command first to create 3D sketch geometry. I believe my dialogue may have been a bit misleading in my last video. I apologize for that.

If you include 3D geometry (create projected sketch geometry) prior to creating sketch figures such as lines or splines, then the sketch geometry will create constraints automatically during creation or "snap" to the projected sketch geometry. See the below video for details.

The video also highlights a work around that you may be able to employ if you are making 3D splines tangent to straight edges.

This is as far as I could get today, but I'll be back tomorrow! 

Cheers,

[cekuhnen]

Thanks for the video. It quite honestly seems that I do not fully understand how the constraint and sketch workflow is best used as it is new to me. Knowing the idea behind them and having years of experience is different. I followed a canoe Inventor tutorial and was able to translate most of it to Fusion. Very interesting while in Alias I would be faster and yet have a parametric design.

But the tutorial and your video showed how you have to pre-think your design steps differently.

Maybe the help section should be more filled with such basic shape modeling tutorials because once you understand the logic working with it is easier.

[cekuhnen]

I just realized something why I rely on snapping so much. When I work in
furniture with multiple elements and things are still in
the exploitative phase setting up and using constraints is time consuming
and can also be wasted time.

Also most I noticed that most 2D sketch tutorials and videos always deal
with the fact that we know what we are going to build.
But in most cases you might not really have any clue about data etc.

This is why just snapping to other sketches without the need to use
constraints will really be extremely helpful for
concept modeling.

[innovatenate]

Using that coincident constraint method in the video above, you can then move the end points of the tangent handle to increase or decrease the size of the tangent handle. This will increase/decrease the curvature of the spline at that specific fit point.

In this next video, I show a method for aligning Spline Fit Points between two different sketches. It does take a little extra work since you have to build some construction lines but you can get alignment along the default axis fairly quickly.

In Inventor, there are two different sketch environments, 3D and 2D. Certain constraint tools are enabled for each environment. I really like the ability to have 3D sketching and 2D sketch in a single environment in Fusion 360. However, it seems that some of the usual functionality of constraints and 3D sketch figures may not be implemented for 3D sketch figures at this time. After all, 3D sketch is fairly new, only ~6 months old in Fusion 360.

For example, I note that I cannot add general dimensions to tangent or curvature handles of 3D spline curves. I also note that some constraints are not enabled when selecting a combination of 3D sketch geometry.

• selecting a Tangent Handle of and a 3D sketch line : perpendicular, parallel, equal, co-linear, etc are not enabled in the Constraint dialog
• selecting a 3D line and a 3D spline : the perpendicular and tangent constraints are not enabled

Having these constraints available would make working with 3D sketch figures a bit easier with the existing sketch and constraint tools. I think it would be interesting to see some video of your favorite alignment or snap tools in Rhino for comparison. Please share if you have the time. 

I hope these helps. Let me know if I've overlooked anything.

Thanks,

[cekuhnen]

I made you two videos showing you how the sketch engines work in Rhino and Alias compared to Fusion.

sketching in rhino:
https://drive.google.com/file/d/0Byzv_NlyKp_2NThJVk1Idzh3OUU/edit?usp=sharing

sketching in alias:
https://drive.google.com/file/d/0Byzv_NlyKp_2ZkJSYjZUUk9KSUE/edit?usp=sharing

I hope this explains a little the different approach to how you structure your design and how you can work/

[cekuhnen]

Here is a quick screencast showing Alias's design history in action

https://drive.google.com/file/d/0Byzv_NlyKp_2R3ZXdF9SRnhlNnc/edit?usp=sharing

[cekuhnen]

Also I forgot to mention this, Alias besides the curve tool also has so called keypoint tools which are close to the sketch engine in Fusion offering you line arc tangent/perpendicular parallel tools and you can join elements to create relationships.

They are ideal when boxing out proportions as they also have length information and providing you with guide lines to snap to.

For mechanical parts quite ideal and can be mixed with other curves.

here is an older lecture recording:
https://www.youtube.com/watch?v=-L26IiBM33w

[banshee10]

So my feedback is that there is no way, as in none, zero, not possible, that we could figure this out from the documentation. Please add it! (Or point me to the place that could have led me to figure it out on my own)