Creating and using Aligned Views

[LibertyMachine]

I've encountered something that's stumping me: How to create and used a perfectly aligned view, relative the the plane that I want to work in. Screencast attached for details.

I know how to use the "Look At" button, but that's not giving me the orientation I need, as it skews the sketch plane. I know how to create a Named View and update it, but that still doesn't solve this, since I can't align my drawing canvas correctly to the plane I am working on. 

[HughesTooling · Accepted solution]

@LibertyMachine For just an aligned view, create a joint origin and snap it to the centre or corner point of the face and rotate it to match the part. Now select look at and select the joint origin and your view should match the part, create your aligned view. 

To get sketches aligned, create a component then make its origin visible and create a joint. Select the components origin then the joint origin you created before for the aligned view. Now with the component active create a sketch and select one of the components origin planes and align the view using the named view. See attached example.

Mark

[LibertyMachine]

Alright, that is totally not the workflow I was expecting to find, but it does get the job done. Not fond of the many steps to go through, what are your thoughts on it? In the software you work with often, how do they handle something like this?

[HughesTooling]

I create a component for each body so having some rotated is not a problem, for performance it's a good idea to either ground the component or fix it with a joint. As for the view alignment I don't really care about it, the only time it's a problem is making 2d drawings but the named view works for that. One problem with named view is if you need to rotate or move the part you can't edit the named view and repick the joint origin. Really named views need to work like a joint origin you can attach to a face and have it follow\update. I've brought this up a few times as a weakness working with assemblies in Fusion and making 2d drawing but never got any interest from support.

In more traditional solid modelers where you have parts in separate files the drawings would be made from the individual files so their origins would be used. You'd generally design in the individual files so the parts are aligned with the axis. This is similar to my example file, create a component and the first feature is adding a joint to align the component then create the sketches and bodies.

In your example did you rotate the body or the component? If you rotate a component and use it to create a subassembly any components created in it will have the same alignment and origin so if you're creating a pair of soft jaws I'd create a component and use a joint to position and align then create 2 components for the jaws and make the whole subassembly a Ridgid Group.

Mark

[LibertyMachine]

That was my issue then; I rotated the base imported feature before turning it into a component. I will try to be more mindful of that in the future, thanks for pointing me in the right direction Mark!

[KennethOfLeesburg]

You can argue about the efficiency of the workflow, but this is really powerful for 2D Drawings.

If you create one part per “file” (i.e., per design) then none of this matters.  But part of the power of Fusion is that you can co-create several parts in one (admittedly small) assembly.  If you change the details on one part the details of a mating (or otherwise matching) part will change automatically to accommodate the progenitor change.

But if you take advantage of this capability you end up with a result that is hard to convert into 2D drawings.  But this is only because you lack the relevant views, which you really can’t do precisely by hand (though it seems you can use the API).  So, at the end of your design process you create a group on the timeline for other purpose than to create a collection of useful named views.

The only PROBLEM was that it just didn’t work for me.  If you click the Look At button (on the viewing tool bar near the bottom of the drawing area) and then click a face (or construction or sketch) it will automatically align the view with the indicated face.  But it doesn’t allow you to select a joint origin.  The TRICK is to do it in the reverse order.  Joint origins must be selected before you push the look at button.  For all other entities you can select in either order.  Apparently, my habit is to push the look at button and then select the entity.

[HughesTooling]

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@KennethOfLeesburg wrote:

  The TRICK is to do it in the reverse order.  Joint origins must be selected before you push the look at button.  For all other entities you can select in either order.  Apparently, my habit is to push the look at button and then select the entity.

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Hadn't noticed that, don't need it that often so not sure if something changed or like you say I selected the joint origin first. 

Also should thank you for bumping this thread as I just tried editing a named view and it is now possible to edit to a new orientation. In the past when you right clicked a named view to open the menu with the update named view option it would rotate to the exiting orientation and clicking Look At would end the command without updating. Now if you select a "Look At" a face or joint origin you just need to right click the named view you want to edit and select "Update Named View" from the menu. Don't know when this was fixed!

Thanks Mark