Joint : make to surfaces stay parallel in an assembly

[cl3m.germain]

Hello,

I am trying to keep parallel two surfaces of 2 components of an assembly. In the pictures, this is the 2 selected surfaces (in blue). I would like them to stay parallel whatever the position of the other joints is, without those surfaces to be in the same plane.

If I use the "alignment" function in the joints menu using 0° angle, i have to set an offset value. But i can't because the two surace are going to slide on a vertical and horizontal axis on a circular route and the distance between them is going to vary all the time.

Any suggestion on how i can proceed ?

Thank you

Clémence

[innovatenate]

Below are a couple of screencasts you may find helpful. I think what you're looking for is the planar joint:

However, just in case, here is another screencast showing how to use the slider joint:

I hope those help!

[cl3m.germain]

Hello Nathan, thank you for your answer.

I've already tried those solutions, but my problem is that i would like to be able to combine the planar and the slider constraint. The 2 surface have to remain parallel all the time, but with no other constraints at all : no offset value, and no slider axis. Or, the possibility to say that the surfaces can slide on all the directions X Y Z in the 3D space.

There is this function in Solidworks, to keep 2 surfaces parallel and be able to move them in any directin after that. Is it not possible with fusion ?

[TrippyLighting]

It can be diffcult to leave that Solid Works frame of mind behind when working with Fusion 360.

The intention of the joint system in Fusion 360 is to work as physical parts would be joined in the real world. The sceenshot you posted above indicates that your current design might not include the geometry/components to constrain the movements. You'll find that once your design has progressed to the point that you have all these components in place that using the joint system in Fusion 360 becomes quite natural and intuitive.

Having said the above I personally believ that the geometric constraints (mates) Solid Works uses and the joint systems in Fusion 360 are not mutually exclusive but could perfectly coexist. To quickly evaluate an earlt prototype of a design the traditional mates can be very helpful.

[cl3m.germain]

Ok, i see. My problem is that i have all the elements for my design already, but i wanted to copy the effect of the gravity : the surfaces i was trying to constraint will always stay parallel to the ground in real life because they are the heaviest part, and the joint above is a sphere/ball joint, so with the weight of the component it should not be able to rotate the way it does in my assembly right now.

But maybe if i try to add other "support" components or axis i will manage to optain what i wish. 🙂 

[innovatenate]

Here's a short screencast that shows how to utlize Joint Origins to set up a Slider+Planar Joint quickly. I think this will help accomplish what you're after. Let me know if you have any questions!

Thanks,

[cl3m.germain]

This might help, but i can't see the screencast..

Can you send it again ? Thank you 

[innovatenate · Accepted solution]

So Sorry about that!  I don't know what happened! Here you go!

Thanks,

[yebyps]

Yeah that works OK, but it is a workaround which can be done in one operation in Solidworks.  I don't think it's very direct to say that Fusion is aiming for a real-world functionality and imply Solidworks isn't.  The parallel plane situation I'm trying to set up is real-world - it's on a product which has been in production for a few years which was designed in Solidworks and which I'm now trying to rebuild in Fusion.  Please can Fusion just learn from user feedback and build in what is a common and useful function? 

[TrippyLighting]

---

@yebyps wrote:

Yeah that works OK, but it is a workaround which can be done in one operation in Solidworks.  I don't think it's very direct to say that Fusion is aiming for a real-world functionality and imply Solidworks isn't.  The parallel plane situation I'm trying to set up is real-world - it's on a product which has been in production for a few years which was designed in Solidworks and which I'm now trying to rebuild in Fusion.  Please can Fusion just learn from user feedback and build in what is a common and useful function? 

---

If you have  specific problem that you need help with, then pease create your own thread and state your case.

[yebyps]

It was the same problem as stated above :  " trying to keep parallel two surfaces of 2 components of an assembly. "  However by studying your workaround I have actually managed to recreate the kinetics of the product, which is a treadle pump.  It took me all day, but I'm there, and I've learned quite a bit about the way Fusion handles joints. Cheers

[giorgio.demurtas]

Hello,

I have motor which feet should stay in horizontal plane whatever is the position if the shaft (which depends on the rest of the machine).

It seems that to accomplish this constraint I have to follow the suggestion of innovatenate (make two joints, one vertical slider and one horizontal planar).

It would be nice if Autodesk could add an option for the planar joint where there is no constraint on the direction perpendicular to the plane.

[therealsamchaney]

@innovatenate Thank you, that's certainly a creative workaround, but is this really the "correct" way to achieve this in Fusion 360?

It does seem very clunky or hacky compared to SolidWorks which as @yebyps correctly stated could be achieved with a single mate. Having to create this mysterious empty component is very counterintuitive and also leaves you with an otherwise useless component that clutters up the browser.

I don't see why constraining components should be any different than constraining sketch elements. You're just removing degrees of freedom of one object with respect to another object / reference frame. I agree with @TrippyLighting that it would be great if Autodesk could add something similar to SolidWorks' mates alongside the joints. Really, I would just like to have a little toolbox of simple 3D constraints I can apply. For example, make a face from one component parallel to an origin plane of another. Or, maybe make an edge of a component colinear to an axis. Then I can carefully build up my constraints until I have just the degrees of freedom I desire.

The joints are just too specific and oversimplified, there's not enough control. It's like trying to use Windows Movie Maker when I need Adobe Premiere. Fusion already has such a robust set of constraints in the sketch environment, I would think that the team could surely implement similarly fine and specific 3D constraints for  components in an assembly.

[innovatenate]

You can use a as-built joint today to simplify that workflow (feature added after the above video). Attached is an example, no extra components necessary. 

Joints should help to define all of the necessary degrees of freedom with one command instead having to create multiple constraints, etc.. If you want a slider (like in my attached example, you only need 1 joint versus two mates). You could constrain an axis and edge together like in the example you mention, but you still have a degree of rotation to worry about.  

There's lots of great features that joints have that constraints don't.

Examples:

• Creating joints with a timeline considerations (when geometry is simple)
• Select the mid-point of a cylindrical face to define a joint (so your rotating parts are aligned). hint hold down CTRL or Command to "lock" a face when selecting the origin to define your joints
• Selecting the centroid or center of a surface to define a joint.. (easily center things without reference/work geometry)
• Creating a joint with origin at the midpoint between two parallel faces.

If you're coming from constraint based assembly, joints take some getting used to, but worth the learning curve. In Inventor, both constraints and joints exist side by side.

FYI - That screencast is vintage circa 2016. As-built joints were added to timeline modeling environment after that. Still nice to get a comment/question on it. 😃

Hope this helps! 

[yebyps]

When I open your file, I just get one component with a slider joint, not two components which keep chosen faces parallel. What am I missing?

[therealsamchaney]

Sorry I should have made that more clear. For the example file, I want to make the front edge of the cube to be parallel to the X axis of the main assembly. This along with the slider joint I already made (which only allows it to rotate about Z) would theoretically make it fully constrained.

[therealsamchaney]

Hi Nathan, thank you. Yes I know these things and I do see the appeal of joints and while they do cover the majority of use cases, there are still some edge and corner cases (pun intended) that they don't and there unfortunately isn't any other tool in Fusion 360 to address those.

That's why I wouldn't want joints to be removed, I just want simple 1 DOF mates/3D constraints to be added to fill in the gaps that joints miss.

This case for instance, I don't see how an as-built joint would help me. Those are for components which are already in the right place and don't need to be moved. I'm talking about a component which is not in the right place, and does need to be moved in order to make one of its edges parallel to another component's edge or axis, and as far as I can tell, there is nothing in Fusion 360 to achieve this. As I've said, Align is close, but it can't be used in conjunction with joints so it doesn't work in an assembly.

[innovatenate]

Thanks that helps. I see your and everyone's points. I'll submit this feedback to research team. 

One thing I didn't mention in the previous posts is the reorient feature of joint origins. If you reorient your joint origin that will give you a place in "space" to work off of with the existing joints. 

You still can't quite achieve what the OP was looking just making a surface parallel to plane or a edge parallel to an axis, but there are some close results that may work for a lot of cases. Another example is attached just in case it helps. 

[yebyps]

I'm not sure if somebody has already said this, if so, apologies, and anyway I don't know if it goes anyway to solving the parallelism with edges etc, I haven't tried that yet. But for components it seems to work quite well. 

You have two components. Each has at least one planar surface which you wish to be parallel to the other planar surface on the other component.

If the planar surfaces are not initially parallel I think you have to align them (modify/align). When you do that they snap together, as the align surface command doesn't have a distance option (which would be useful). Having done that though, you can use the Move widget to distance one component in any orthogonal direction so the surfaces are still parallel though as yet with no relationship.

Then Assemble/As-built Joint. It asks for components to be selected. Select one component then the other. Then select the Joint (in the Motion section) type as Planar. The OK button is still greyed out, but if you click one of the surfaces it animates showing the degrees of freedom: distance and revolution, and you can click OK.

If you ground one of the components you find that the other component can be distanced but only rotated by keeping the chosen surfaces parallel. If you unground both components and rotate either, the other component will rotate to keep both surfaces parallel.

This is pretty simple to do despite my lengthy explanation and it seems good enough for the time being.

[queezz]

Autodesk Inventor has both joints and constraints. Why there was a decision to remove constraints from Fusion 360 evades me. Yes, joints are quite helpful, but would it hurt to have constraints as well? Or then Fusion will be more like Inventor, and Autodesk wants to have less compatibility between the two? Is this marketing a solution?