Rectangle with Round Corners?

[Anonymous]

VERY new to F360 ( and design in general ) and am about to pull my hair out.

I am trying to model a very simple makeup case cover for my daughter.  It is a very basic rectangle with rounded corners.  However:

The corners at the bottom of the rectangle are much more rounded than the corners at the top.  It is actually this cheap case:

http://www.google.com/imgres?imgurl=http%3A%2F%2Fi.ebayimg.com%2F00%2Fs%2FMTAwMFg0OTc%3D%2Fz%2F0KsAA...

I have been searching for about 30 minutes now just create a rounded corner and am utterly lost.  Any help would be much appreciated!

[jeff_strater · Accepted solution]

Don't tear your hair out!

There are a couple ways to handle this:

1. start with a sketch, draw a rectangle, use the Sketch Fillet command to create the rounded corners.  You will need to use the command twice to get the different radii:

invoke skethc fillet, and make one corner, choose the radius you want:

then, in the same command, select the other two lines for the second corner of the same size:

and hit Enter to finish.  Restart Fillet, then do the same for the bottom two corners:

and this is the result:

Then, use Extrude to give it thickness:

2. start with a Box, and use solid Fillet to add the corners:

create a box:

then invoke Fillet from the modeling menu, and choose two edges:

type in the radius you want, or drag the blue arrow:

then click OK.  Start the Fillet command again, pick the other two edges, and use a different radius:

Both methods will end up with similar results:

Good luck with your Hello Kitty case.

Jeff Strater (Fusion development)

[Anonymous]

Thanks a ton!! 

I was missing the fact that you can select a "corner edge" for fillet!  

[CLmoss]

Dr. Strater,

you hit the nail on the head again.  This is exactly what I need to know about right now.  

You must be a mind reader!

JM

[cekuhnen]

@Anonymous

Welcome to fusion a wonderful app - ask -length of questions and we will help you.

jeff mentioned everything but as a tip of advice I never fillet sketches I always extrude sharp edges and then use the surface (patch/model space) fillet command

to round the edges.

this way you have fillet features you can adjust and tuned off/on

plus your sketches remain nice and simple.

[CLmoss]

Wait, I cannot get Approach #1 to work.  I cannot get the Sketch Fillet tool to grab the edges.  I don't even see a dialog box.  

See Body drawing Attached. 

JM

[CLmoss]

Sounds good to me.  Can you upload a graphic or something? 

JM

[CLmoss]

Never mind. I figured it out.  Thanks!

[Mike6158]

I'm glad I'm not the only one that was stuck. Not any more thanks to this wonderful resource

[TrippyLighting]

One thing that was not covered in this thread is that you should try to fully constrain and dimension your sketches at the very latest before you summit something to manufacturing, regardless  whether thats the 3D pinter on the kitchen table or the shop floor of a manufacturing facility.

As such the rectangle Jeff started should have had a reference to the sketch origin.

[Mike6158]

Thanks for the heads up. I'll see if I can find a way to do that. I have a very small project that I want to try to do on my Othermill. It's basically a 29.50mm x 63.5mm x 2.00mm aluminum cover. 3mm radius on the corners and 4 holes drilled for attaching it to an extruded aluminum case. I'd like to mill some holes in it to accept power connections (Powerpoles if you're familiar with DC connectors). I have recreated the cover from mfg drawings. Sketch only, no CAM (that's another hurdle). Now I need to add the "openings". It has taken me two hours to get this far. Good thing I don't have to make a living doing this!

[CLmoss]

I don't really understand the argument for constraining a drawing.  Maybe it is just the jargon I don't understand.  If you make a 3D drawing to the specs you want produced, that should be it.  It was it when I did in with a paper and drawing pencil.  Maybe what you are saying is that you should provide to a shop not only a 3D STEP file, sheet or otherwise, but to have a dimensioned drawing along with it.  Like a PDF.  However, with a Model or Sheet Metal, you can use Measure to check your dimensions without the dimensioned PDF.  Where does the word or concept of Constrained come in to this?   If I draw a 4" x 4" box, that should be considered constrained.  

If this is not true. Then maybe you can explain to me the difference.  What is Trippy talking about.

It was 107F here today. 
Jim

[TrippyLighting]

Yes, this is likely a terminology issue at least to some degree.

So let me clarify the usual use of this terminology, which is also reflected in the Fusion 360 user interface:

Sketch

Aside from T-Splines and the primitives in Fusion 360 (Box, Cylinder, etc.) sketches are the only way to create 3D geometry Fusion 360. They are mostly created to serve as the basic outline of geometry.

Model

A model, in Fusion. 360 also often referred to as the design constitutes 3D geometry. This is NOT a drawing!

Drawing

This is a technical drawing and in Fusion 360 can be created by making a drawing from a component group (assembly) or a single component. Many people unfortunately use the term drawing when referencing a model.

My earlier comment is related to sketches only.

As the elemental building blocks, if these are not fully defined, meaning all sketch elements are properly constrained and dimensioned so they cannot freely move, this can easily break a design. For a single 3D printed object this might not of much importance but when you build a manufacturing machine with hundreds of components, under constrained and not fully dimensioned sketches can lead to very costly disasters, when things don't line up.

Fusion 360, depending what screen background (Environment) you use choose, colors fully defined (constraind and dimensioned) sketch elements differenty to let the user know that this is fully defined.

I often use "Infinity Pool" and there sketch elements turn black.

[CLmoss]

Thanks Trippy.

That was very helpful. 

Jim 

[CLmoss]

Trippy, 

I see a possible problem here, at least in my case.  This concerns the k factor as well as things like the corner radius details which are dependent, as we discussed before, on the quality of the tools used by the sheet metal shop.  As I understand my function as a designer is to assume a value for these and incorporate them in my design.  If I did not, then there would be no sheet metal design.  Then the shop takes my design and creates their own design which they will use to produce the parts.  This design must match what I created in my design.   

So you have two designs then, mine and the sheet metal shop's.  If "all sketch elements are properly constrained and dimensioned so they cannot freely move", there is still nothing to stop the new sheet metal shop design from having a different k factor and corner relief from my design.  As I understand it, selecting a k factor has an influence on things like bend allowance and bend deduction.  How does constraining our drawing help us when we transition from our design to the shop who will make the parts for us.  We want the parts to be exactly like our design, but we need to give the shop some freedom to change it.   

It is this situation that troubles me at this point in my design to manufacture process.  

Jim 

[cekuhnen]

@CLmoss @TrippyLighting

The reason for fully constraining a sketch is simply - unlike cad apps that do not use a solver Fusion uses a solver and thus the sketch is like a house of cards.

Think of constraining like stabilizing your sketch so when you edit a value the solver will adjust the sketch you want and not how the solver might think.

In Alias Rhino and such where there are constraints and I can move something of a sketch and nothing else will be adjusted or influenced.

On the other side as long as you know what you do not everything has to be also constraint.

it is a pain to adjust a design when having to always adjust dimension values (face palm process) vs push n pull spline fit points to much faster evaluate how

sketch changes will result to surface changes.

Sometimes instead of dimensions I just use the lock icon so parts of sketches cannot move.

This is were traditional parametric sketch modeling ideas collide with free form surfacing workflows and each on thinking they are superior.

You as a user have to make the call when what tool and function will be best used without blindly following some CAD ideologies.

Constraints in general can also be very helpful when you open a sketch and you see two lines have a 70 degree angle constraint.

I instantly see that. If no constraint is there I would have to measure the angle first.

So for readability the idea of constraints is pretty amazing - it also replaces functions like rotating something in a sketch.

In your example with a 4" x 4" square you can draw a line to 4 inches horizontally while using grid snapping

or

you can draw quickly a square like shape, then add 4" dimensions to the lines and then to horizontal and vertical edges add vertical/horizontal constraints

so that they never rotate.

also the center point of a sketch is for parametric modeling important. for example for sweep along a path you can make a construction plane that flows along a path

and where the path and cPlane intersect is always the sketch x/y 0 point.

[TrippyLighting]

It is fairly common practice in many areas of manufacturing to adjust the initial drawing to match manufacturing conditions.

Simulation tools sometimes can help to ease the need for that but there are areas of manufacturing that are very difficult to simulate with reasonable efforts and budgets.

[cekuhnen]

Yeah and the fact that designers and product - manufacturing engineer work with different cad apps also does not help.

Today we still are kinda split between freedorm surface and parametric solid/surface modeling environment for most of the time.

[CLmoss]

I thought Fusion 360 was a CAD/CAM program?  They advertise it as such.  

Also, I have never heard the term Solver with relation to Fusion 360 before.  

I don't know what you mean by "Fusion uses a solver and thus the sketch is like a house of cards".

Please explain

Jim 

[cekuhnen]

@CLmoss

Fusion sketch engine uses a solver to adjust sketches like when you add a length dimension and change the value it scales the line.

A dimension can also be shared. A square can have one dimension for an edge and that dimension once changed will be used for all

other 3 edges.

In Rhino Alias or such you cannot do this. You maybe have the ability to set the length of a line because it treats a line as an object.

but the rest has all to be done by hand via common tools like move scale rotate trim extend and such.

Also the term CAD is I find to day quite used in the wrong context and often used to give justification to their cause.

CAD sounds so industrial standard but guess what even SketchUp can be considered CAD as a computer aids me in my design.

The main difference is how Fusion works vs lets say Rhino.

In Rhino you can create 3D freeform curves and from those curves create surfaces and use typical NURBS modeling tools to manually

create the 3D model you want.

In Fusion follows more the idea of 2D sketches that can be constrained and offers surface and solid modeling tools where everything if

logical can be parameterized and is stored in a design step by step (timeline).

Technically speaking Rhino follows more a workflow of philosophy designers use and Fusion rather follows an ideology engineers use.

Some people see it this way - but even that I found out dated.

The freedom of Rhino to sketch in 3D where ever I want is liberating considering that Fusion is incredible weak at it.

Because in Rhino there is no timeline or construction history I can simply model where ever and when ever I want.

There is no feature relationship I need to be aware of to prevent feature references to break.

The down side is when you want to edit a design you kinda have to manually remove parts, untrim surfaces, resurface, trim again stirtch and and and.

Fusion on the other side with the more 2D sketch modeling feature based approach only offers usable 2D sketches however unlike Rhino offers

me to create interactively reacting sketches that I can deform or influence and with the ability to also adjust parameters of modeling features I can change

the design rather via adjusting values than deleting parts and modeling it again.

However that power also means you have to be very careful about where and when do adjust the timeline.

One of the major advantages of apps like Fusion is how the surface modeling tools in general work. Direct Modeling in something like Fusion is amazing

with heal functions and such. For example in Fusion you can select a filleted edge delete the fillet and you will get back the original sharp edge you filleted.

In Rhino you will open the surface because you just removed the fillet surface.

Alias in that area is kinda a hybrid.

If offers a construction history with full 3D sketches and very powerful surfacing tools that defeat Rhino hands down. A fillet edge can be adjusted when ever needed

and the surfacing command can be even removed - giving you back the original untrimmed surfaces. There is also no strikt top down (timeline step by step) requriement

when you can adjust surfaces. But Alias comes with its own share of problems (class a surfacing is hard - Alias offers 0 solid tools).

3D software and how you can work today matured and expanded in the past 15 years in amazing ways. However there are still too many old school / traditionally thinking folks

out there that claim it aint the industry standard and thus revolt against innovation.

What makes Fusion so great is not the tools (in that regards it just offers typical tools everybody else offers to (and better)) but how the software ties all the tools and environments

together and provides from my point of view a superb collaborative tool. Collaboration via the cloud that is really an area where Fusion is pretty stella at!