How to find the center of an uneven shape/sketch

[ovisopa]

Hello everyone,

can anyone tell me how I can make a point or find the center of an uneven shape ? I want to draw a rectangle around that shape, having the shape exactly in the middle, the easiest way for me was if I could have a dot in the center of it, and than start a CENTER RECTANGLE from that point.

Using the middle constrained I couldn't select the entire sketch, to have it in the middle of the rectangle, maybe I don;t know how to use constraints on this sketch.

[daniel_lyall]

The easy way is to draw a construction line from the top to bottom constraining it to the center then doing the same from left to right. example of this attached.

Or you can places a sketch point rufley in the center, click on the point and select horizontal vertical constraint then hold shift down then move the cursor along a side when the center icon pops up click on it, that will lock the point to the center of the line then do the same thing along the top if you did the side first.

If you wont to do it to a body you click on inspect then select center of mass then click on the body.

There is a script in the API section for doing a relative center point to an object, but that's for eyeing it in relative to something, it was requested for it to be selectable and added into fusion but it has not been done yet.

[daniel_lyall]

Here's a rough screencast showing useing two line or a center point 

[ovisopa]

Daniel, I watched your video but I need to watch it again as I think you are getting the center of the rectangle (with rounded conrers), I wanted to have a point at the center of the internal shape, which is a irregular one, and doesn't have straight lines at the edges. So is your screenshot showing how to place a point at the center of the  irregular shape or at the center of the rectangle ? I will post back later, I almost finished the cutting die in this file, I just need to fine tune the blade sharpness, the internal chamfer needs to be a slightly deeper

Thank you anyway for your effort, and excuse me if in your video you show exactly what I wanted, but I didn't understood what you did, this is why I told above that I will watch the video again - to understand every step you made. Quite a lot of steps to align something at the center of another object 🙂

[mavigogun]

You already have the center of one axis- the mirror plane -so you're half way there, right?    All you need now is a vertical line along that axis, starting at the existing point on the upper segment and reaching the lower extent of the lowest segment.    A horizontal line bridging the tips of the downward curved projections would be a great help for locating that lower vertical extent; were there already a point located at the bottom of those curving projections, the next step would be super easy, as you could just snap the horizontal line to that point.   But there isn't, so- draw a horizontal line some distance below and extending beyond the limits of your existing elements; use the move command to slide that line right up to the tips of lower curve.   You'll have to magnify as dictated by your tolerance demands, assure there is contact between the new horizontal line and your curves.    Once so positioned, draw a line along the mirrored axis of your splines, starting from the center upper curve of your form, ending at the new horizontal line.    The center of this last line provides the location sought, easy-peasy, lemon-squeezy.

Forethought when sketching saves much work- "hey, I'm gonna need to find the center of this thing later- how can I sketch to make that task easy?"

Fundamentally, you're trying to write a poem without a vocabulary.    With Fusion, there are usually many ways to confront each challenge- we might have contrived construction planes, located the intersection, for example -but there is no place for consideration to start without a basic familiarity with the tools available.    At this juncture,  "I'm going to learn ways to find or position the center of sketch elements" is a realistic goal; "I'm going to design this part I need" isn't- without a foundation.   You can't cheat experience.

-Christopher

[mavigogun · Accepted solution]

....and a screencast to practically illustrate.   Hope that helps.

[daniel_lyall · Accepted solution]

Here you go @ovisopa I should of ask what part you wanted the center on.

I am doing a start to finish in the screencast sinces you already had half off what you needed with the mirrour centerline I base the start of the topline from the origin, it makes things better if you start from the origin.

With the mirror line if you have it to the height of the top and bottom line the center of the line is the center between the top and bottom line, screencast interferes with some commands in fusion when I places the point you just have to move the cursor along the line to find center not how I did it you can do it that way but you don't have to.

The other ways sinces I don't know if you know it, you have the centerline the total height of the model what's in the drawing, then the center of the centerline is dead center of the model.

I also show how to find the center of the sketch with a rectangle that will be ok to .5mm.

There are more ways to do it, but that depends if you know the overall height of the sketch and how accurate you need to be.

[ovisopa]

Thank you @mavigogun & @daniel_lyall for the screencast, really appreciate the effort of anyone that is spending his time to help others learn this software.

You both show me similar ways on how to find the center of of an irregular curved object, but sincerely I didn't expected the method you showed in the screencasts to be the best / only way to find the center of an object.

On the parts I usually mill, there will not be any accuracy issue because I manually place a straight line as close as I can to the irregular object side, and then another line on the opposite side, but on all other software I worked with (design,cad,cam) there ware tools available either to place one object to the center of another, or to automatically create a rectangle with object extremas (hope this is the right word to use, I mean the automatically generated rectangle will fit exactly the irregular curved object, no gaps on any side) 

So, in Fusion 360, there is no such tool, to automaticall ?

PS. I almost never have to draw the parts I need to mill, I always get them as DXF files from clients

[daniel_lyall]

If the center of mass was selectable yes there would be, but no it's not yet.

The only way would be your clients adding a center point in.

[mavigogun]

"So, in Fusion 360, there is no such tool, to automaticall ?"

'Fit this body/component into a primitive' at a specified tolerance?   Not that I know of- you might suggest it at the IdeaStation:

https://forums.autodesk.com/t5/fusion-360-ideastation-request-a/idb-p/125

[ovisopa]

I added now a new post to IdeaStaion as you suggested, hoping to get some votes from others, as I don't think the solution you showed above should be the way to find the absolute center of an object

Please vote up 🙂

https://forums.autodesk.com/t5/fusion-360-ideastation-request-a/center-automatically-a-curved-sketch...

[Anonymous]

Hallo @ovisopa

Yes there is a way to get a 100% exact center point of a shape!

First of all you are going to fix the existing uneven shape. After that you are going to create points where you think the outer most points are. After that you are creating a new center point rectangle and do a coincident constraint to the outer most points. IMPORTANT: Then the rectangle has a constraint to your uneven shape. When you then drag a line of the rectangle and push it to the outer direction of the shape it will actually get "tangential" to your uneven shape. I hope this is understandable.

After you have the center point you can create your surrounding rectangle. As you see in the picture below, there is a dimension with size 4mm and it automatically says that on the other side it is also (4.00)mm .

Here is a close up of the resulting center points of your U shape and the rounded box.

Last but not least here is a screencast!

I hope that helps!

Greets Fabi

[Anonymous]

Sorry forgot to attach the resulting file. Here you go.

[etfrench]

What's new in the Sept 6 update implies tangent can be applied to a spline.

Apparently you weren’t able to apply a tangent constraint to a projected curve and an elliptical curve. A circuit breaker must have tripped somewhere. We went back and turned it back on.

Unfortunately it doesn't seem possible to make anything tangent to a spline.  My workaround is to export the sketch as a dxf, then create vertical and horizontal lines tangent to the spline in a 2d cad program.