how to align the centers of two bodies

[rms_adsk]

Hi, I have two bodies as shown in the image below. There is a box and an rounded shape. I want the box to be centered on the rounded shape. I cannot figure out how to do this - I can snap to corners and planes, but I can't seem to create any kind of midpoint snap points. Any suggestions?

[lure23]

True. There seems to be either horizontal or vertical center point alignment, but not both at the same time.

i.e. once moving the circle mid point left/right across the square, a green dashed line appears. When moving near the center of the square, a similar green dashed line should arise also vertically.

[karyeka · Accepted solution]

For bodies, I think this is a good requirement, we need a easier way.

However, one of the ways to achieve the result is by using Joint Origins. If I place joint origins exactly at the points I want to align (centers in this case) I can then use align components to align.

Please check the video - http://www.screencast.com/t/Q5oxMSC6

Steps in short -

1. Create components from bodies

2. Create joint origins at the centers of the bodies using between faces

3. Select joint origins in browser (ctrl on windows to select both the joint origins) and right click to select align components

Does this solve your problem?

Regards,

Anand Karyekar

Fusion360 Development

[lure23]

Hi Anand, 

while using joints to make such connections has been discussed elsewhere - and is a decent solution - this was regarding two 2D elements within Sketch mode. I think you overlooked this, since you are suggesting "converting bodies to components".

I think there's very much room for confusion in Fusion 360, currently, because many of the basic concepts are not clearly defined (or so it seems to me as an incoming user):

- it seems I'm actually able to attach joints to 2D sketch elements. Why would I want to do this (= is there a use case)?

- I can 'move' (right click menu) when 1..n 2D sketch elements are selected, but it doesn't do what I want (= move the selected elements). Instead, it selects the whole sketch and starts moving it in 3D.

There may be more of similar cases (i.e. the menu thing I posted earlier today in IdeaStation). It shows that Sketch just "is there" but its role as a supporting actor to the Sculpt and Model workflows is not clear. It tries to get center stage, which imho it shouldn't.

How does this sound to you others, especially Autodesk UI designers? Please help me see the consistency here, or fix the product to be more consistent. Sometimes, *restricting* the user is just fine. I think we should be somewhat restricted when using a Sketch tool.

Moving in Sketch mode. Notice the three axes. Before right-clicking 'move' only the rectangular area was selected.

[karyeka]

Thanks for the comments.

I think the original question from rms_adsk was about bodies (thats what the post and the title says). Sorry, if this is about sketches.

Regards,

Anand

Fusion360 Development

[rms_adsk]

OK, using the joint thing worked to align the objects. It is a bit confusing but I figured it out...

Here is my next (related) problem though. I took the top of my deformed-cut-sphere object and projected it into a sketch.
The result is an oval shape. Now I would like to snap something to the center of this oval.

How do I do that? There is no snap point right now, like there is at the center of a circle I create in the sketch...

[innovatenate]

To solve the initial symmetry issue, I would recommend using the symmetric sketch constraint prior to the creation of the bodies.

http://screencast.com/t/UWiXACVxEO

However, if you didn't want to go back to the sketch to correct the issue, you can use the measuring tool in combination with the Press/Pull or Move (face) feature to move the faces into the correct position. Please note that you may have to create a sketch point to measure from.

http://screencast.com/t/UWiXACVxEO

As for the snap/center point issue, if the figure is an ellipse or a circle/circular arc, Fusion should put a centerpoint down for you to use. From the image, I would guess that you have a spline figure (projected from another bodies edge), which will not create the center point in a sketch. I would suggest pushing forward with the sketch and create a component with it. Then once there is 3D geometry, leverage the use of a snap (joint origin) in the Joint command to position it.

http://screencast.com/t/rekcyeJgwvf

Not sure if it will, but I hope this helps. Let me know if that will work for you.

Thanks,

[rms_adsk]

I did not start from sketches, I just started with T-Splines objects (that were converted to bodies to do Booleans).

I am coming from non-CAD background, where this idea of doing everything via "sketches" is very foreign (neither Maya nor Sketchup  have  this notion of "sketches"). I can see how it is more precise, but it seems very round-a-bout if my goal is to just do visual experiments directly in 3D...

Anyway, thanks for your help. I now have a much better understanding of the limitations I will have to work around 😃

[Oceanconcepts]

Ashlar Cobalt had a menu tool that could be used on their equivalent of sketch objects (in Cobalt, you could draw lines in 3D space at any time without entering a particular mode).  This was "Simplify Object"  and it would analyze curves- if a projected spline could be converted to an arc, ellipse, or circle, for instance, it would do so. 

Ron

[haughec]

Answers to a few questions:

• "it seems I'm actually able to attach joints to 2D sketch elements. Why would I want to do this?"  Placing joints on sketches allows you to begin creating kinematic relationships between components in a layout skectch before creating any 3D objects.  This will be more useful when we introduce modeling history (when features are assoviative to their sketches).  Currently, I use this capability to create a joint to a fixed sketch that represents an component not yet present in my design.
• "I can 'move' (right click menu) when 1..n 2D sketch elements are selected, but it doesn't do what I want (= move the selected elements). Instead, it selects the whole sketch and starts moving it in 3D."  This is a great observation.  If any sketch objects are selected, the Move command moves the entire sketch.  This is useful when your goal is to move the entire sketch, but clearly not valuable for moving individual objects.  We could consider a revision to the Move behavior - if you're in a sketch, Move could only affect the selected objects.  I'll look into this.  In the meantime, you can just drag the selected sketch objects to move them.
• "Ashlar Cobalt had a menu tool that could be used on their equivalent of sketch objects (in Cobalt, you could draw lines in 3D space at any time without entering a particular mode).  This was "Simplify Object"  and it would analyze curves- if a projected spline could be converted to an arc, ellipse, or circle, for instance, it would do so."  This would be useful.  A few questions:  Do you ever have the need to convert arcs, circles, etc to splines (the inverse of the "Simplify Object" functionality)?  If you performed a "Simplify Object" operation in a history-based modeler, would you expect associativity to be broken, or would you expect the simplified object to survive if the original projected curve changed?

Thanks for the great feedback.

[Oceanconcepts]

"Do you ever have the need to convert arcs, circles, etc to splines (the inverse of the "Simplify Object" functionality)?  If you performed a "Simplify Object" operation in a history-based modeler, would you expect associativity to be broken, or would you expect the simplified object to survive if the original projected curve changed?"

In Cobalt, this conversion broke the associativity (with a warning), and yes, there is also a "Convert To ...." menu command to change one type of line or curve to another.  I found myself using the Simplify version a lot more, though. 

Ron

[lure23]

Sorry, rms_adsk, I immediately thought you were working based on sketches because the brownish square in the original pic. My fault.

[NicolasXu]

Hi rms_adsk,

If one of the bodies has simple shape (box in this case, which has straight edges parallel to origin axis and can easily get the movement distance), I would use Move command (Snap + Measure) to align the two bodies.

Please refer to the video for steps. The center point of the manipulator can be reoriented to the center of the body.

http://screencast.com/t/DGIGu5vYR

Hope it helps.

[rms_adsk]

NicolasXu, one question for that approach - how would I get the height measurement if my object has curved sides? This is what it actually looks like from an angle...there is no straight vertical line to measure along. I guess I could construct some stuff on the two faces and then measure between them, but that seems like a lot of work...does the measure tool have a way to measure along the X/Y/Z axes?

[NicolasXu]

Ryan,

The in-command measure tool support measuring distance between two planar faces, two vertices, etc. (there will be a green line to indicate what distance is measured).

However, for the model with curved sides, I think we may have to construct some plane for moving one body to a base point of another body.

Please refer to the video below for details. It seems we need an easier way to move/align bodies.

http://screencast.com/t/2Fv89HAsNr

Thanks again for letting us know the case.

Best Regards,

[Anonymous]

Hi all,
I know this discussion is quite old, but maybe you can help me.

I would like to know how to center a svg image in to a sketched shape (e.g. a rectangle)?

I hope my question is clear.

thanks

[NicolasXu]

Hi leonid, 

For the svg image you mentioned, were you using the “Insert SVG” command (which is under the Insert group on the Ribbon) to place it into a sketch? If yes, Fusion will generate sketch curves based on the selected .svg file. 

These curves are shown in green, which indicate they are “Fixed” and cannot be moved. To move them, we have to select them all, right click and select “UnFix”. After that, we can use the Point-Point mode of Move command to position it. 

If it's not the case, could you attach the file or some screenshots to show the details so I can provide more specifical approach? 

Best Regards,

[Anonymous]

Hi Nicolas,

I attach you the SVG file. If I want to put it in the middle of rectangle, and "fix it" in order that if I will resize the rectangle, the image will resize too, keeping place in the middle of it.

Let me know.

Thank you.

Leo

[NicolasXu]

Hi Leo,

We can use the Move command to align them, after removing the fix status of the imported curves. However, I didn’t find an easy way to keep the relationship. 

One workaround I can think of is to leverage the Scale command under the Modify group on Ribbon.  We can scale the rectangle and the imported curves together.

Steps:

1. Put the rectangle and imported svg into one sketch.
2. Exit the sketch environment.
3. Invoke the Scale command from the drop-down list of the Modify group on Ribbon.
4. Select the sketch node from the browser.
5. Specify the point and the scale factor.