Align difficulties without reference points/edges

[Helmi74]

Hey there,

i'm still struggling with guidance and alignment in Fusion360. This is something that is generally often unclear in Sketches and other situations. Here's an actual example i'm often struggling with when trying to align objects that don't have a corner/edge that play well with where i want to align it to.

In this case i want to align the cylinder to touch the extended x and y axes - basically i want to align its "surrounding box" (that isn't there) to the origin point of the WCS.

Probably i'm just missing the intended way to do this - ideas?

Thanks!

[HughesTooling]

It's easy to do with a sketch and extrude. If you want it parametric it would be more trouble to use the solid cylinder anyway, coming from a solid modeling background I never bother with the primitive solids it far easier to use sketches that can use constrains, driving dimension and parameters.

Here's an example sketch, you can edit the diameter in the sketch or in the Parameter manager and it's position will update.

Mark

[Anonymous]

There's definitely multiple ways to do this.  Another way I've found that's powerful, especially when getting into complicated assemblies, is using joint origins together with rigid joints.  So say for instance you have a component A, and this cylinder is a subcomponent B within A.  You can create your first joint origin for A creating a sketch in A containing a point, or just turn on visibility of the WCS Origin for A.  Then go to Assemble > Joint Origins, click on the A WCS Origin so the joint origin is placed at 0,0,0.  It will by default have its z axis aligned with WCS z axis, and you can in joint origin dialog box choose to select a different z axis, by choosing that option then choosing a different WCS Origin plane to have the z normal to. 

You can then enter an offset for the appropriate joint origin axises, in my case diameter/2 for x and also y, diameter being a user defined parameter for the cylinder diameter.  Note it's always good to first establish desired joint origin orientation, before entering offsets. 

Once done, the joint origin will automatically go into a Joint Origins folder within A, since the joint origin was defined on a sketch, body, Origin etc contained in A. 

Next create a joint origin defined on the cylinder in B, and joint origins has a handy Between Two Faces type to quickly place a joint origin right in the 3D geometric center.  Finally create a rigid joint between the two joint origins, just being sure you're selecting joint origins (will kind of highlight) rather than creating a new joint origin when making the joint.   The rigid joint will go into a Joints folder at an automatically determined location in the Browser tree based on the components relationships. 

A few additional notes are when wanting to edit a joint origin offset or add an additional offset to a joint origin axis, do not edit the joint origin in the timeline, but rather find it in the Edit Parameters spreadhseet, otherwise parametric equations for the joint origin offsets will be lost, due to a current limitation it seems.  Also, when placing joint origins on a line or edge, the first left mouse click will select the line, then the second click will determine if want joint origin at first end, middle, or other end of the line. 

Jesse

[Helmi74]

Thanks guys,

i know there are some ways for some cases but both of your suggestions don't work for the example that i mentioned in the first post (of course i could rebuild the cylinder easily via sketch but imagine that wasn't just a cylinder but a more complex part/assembly).

[HughesTooling]

There's is an option to add a plane tangent to a surface but it seem to add the plane at a random angle, I can't figure out how you're supposed to use this command for anything useful. There is also add Plane Tangent to face at point this might do what you want but you'd probably need to sketch a point. As long as the planes are added with the component active you can then use align to align with the construction planes.

Mark

[Anonymous]

Hmm, with the joint origins you dont need a sketch, as I described.  If you could provide an example of what's giving you difficulty that would be good.

Jesse

[HughesTooling]

I see you can setup a joint origin using reorient but how can you snap it to the surface of the cylinder without measuring it, on an imported part you might not know the size. Also if you manually enter a size it's not going to update if you modify\scale the size.

Mark

[Anonymous]

Hey Mark, regarding a cylinder, for the first joint origin that will be for the cylinder, just snap it to the center, i.e. onto the cylinder axis.  As I mentioned you can also have it snap to the 3d geometric center of the cylinder, i.e. still on the cylinder axis, using the two face option for joint origin type.  Then for the second joint origin that will be defined with respect to for example the parent component origin, just snap a joint origin to the component origin, realign z if desired (using realign in joint origins panel and one of the origin planes), then finally add proper parametric offsets for the joint offsets, so say for instance cylinderdiameter/2 for the x and y offsets of the joint origin, where cylinderdiameter is a user parameter for the cylinder diameter.  And make a rigid joint between these two joint origins.  Then everything should work and parametrically update nifty gifty.

For imported parts that were not made in Fusion, I haven't tried to see if joints/joint origins will have snapping points.  Also for more complex geometries, may require a sketch to specify the desired location for the joint origin for the part.

Jesse

[HughesTooling]

You need to forget about the cylinder, if you import something with a cylindrical surface you want tangent to face on another part how do you do it the when none of the sizes are known and none of it is parametric.

Mark

[Anonymous]

Hmm I'd have to experiment with that.  All the modeling I've done has been right in Fusion. 

Jesse

[HughesTooling]

I've used a couple of other solid modelers and they have a tangent constraint in assemblies. Most of the assembly constrains from those programs can be done using joints in Fusion, the Tangent constraint seems to be the only one I can't see an easy workaround for. The create Tangent Plane is almost there but it just seem so random!

Mark

[donsmac]

I made a screencast that shows a simply way to align the cylinder the two axis.

Place a sketch on the cylinder to determine a reference point.

Then used the Point to Point feature of the Move Tool to snap the cylinder to the new position.

https://knowledge.autodesk.com/community/screencast/65ec4f4e-e0dd-48de-9769-06de805bab38

[Anonymous]

Two of my favorite construction planes are Plane Along Path and Plane At Angle, which as I'm sure you know are pretty powerful.  So with the former, can choose a percentage of the arc to be placed at.  The arc tangent there will also be normal to the plane, so when a sketch is defined on the plane and Project or Intersect used on the body with a cylindrical/arced feature (I also just tried a STEP import), there will be a resulting line that is perpendicular to the arc tangent that can be used to orient a joint origin normal to the cylindrical surface.  That's one way to quickly and precisely place tangent joints just wanted to mention. 

Jesse

[HughesTooling]

Although that works I don't think it's very flexible. Here's an example from another program, when the tangents are added you can still rotate the part, I think the workarounds will have a fixed point tangent. Here's a Screencast. Note I've waited 45 minuets for the screencast to become available, can't wait any longer so it might not work yet. Perhaps this is one for the Ideastation

Adding a tangent constraint

Then rotating the part with an angle constraint, the tangent constraint allows for rotation.

Mark

[Anonymous]

Hey Mark I'll make a screencast for a method, suitable even  for linked/imported components that pretty much works the same way, using planar joints, contact sets and rests for joint limits.  But need to find my darn microphone.

Jesse

[Anonymous]

Alright found my microphone!  Here's the screencast.  Note I just uploaded it so if experience is any indication, it should be ready to view in about an hour.

https://knowledge.autodesk.com/community/screencast/c3b95437-ee82-4849-81b2-f27cebe773c4

Jesse

[Anonymous]

Hey Mark, I was curious what you thought of this method?

Thanks!

Jesse

[HughesTooling]

Sorry quite busy today and don't have any speakers at work, I'll take a look later.

Mark

[Anonymous]

I'll make a quick screencast with just visual illustration like yours, since I really am curious what you think!  To me this seems like an awesome method very similar to what you've shown with Solidworks, for instances such as where parametric parameters/distances are not known, such as imported parts (natively made or otherwise), yet still want the tangent joints to automatically update when a part is changed...

[Anonymous]

Ok, by the first minute and a half of the screencast, I've established the same parametric dual tangent joints as was shown in Solidworks.  Then for the last minute I illustrate a parametric update of these joints, in this case since one component is linked, I modified its parent component the seperate file, updated the linked component, and showed how the tangent joints update accordingly. 

Align can be used if desired/needed after such tangent joints are made to align the angle of one component to another, but as shown is not needed in most cases.  

https://knowledge.autodesk.com/community/screencast/5247d512-81e4-4d74-96d6-995d00563282

I think this could be pretty big for some uses 😉  What do you think? 

Jesse