A few questions regarding Onshape

IsleofGough

I am just learning Onshape, and I find it intuitive and powerful. I have a few questions though:
1. Is there a way of changing to display to match the material assigned to a part rather than the color assigned? I realize I can add the rendering addin and use that, but Fusion can show a match of the material.
2. I know that constraints can allow animation, but is there a way of animating an assembly the way there is in the animation tab of Fusion 360?
3. Zooming way in to a circle shows a series of lines rather than a smooth curve. Is this just a display issue or can this cause problems with precise alignment and tangents?
4. You can copy a sketch, but can the copied sketch be rotated around an axis (so that you basically are copying a top sketch to a side sketch?
5. Can you extrude at an angle?  I know you can do this in an awkward way by creating a sketch that has an angled line and extruding that and then using the face of the extrude as another sketch plane, but that is cumbersome. This came up as I am trying to recreate the Venn puzzle sphere as a practice exercise.

bruce_williams

I will take a few of these -

3)  you are talking about graphic Tesselation quality - this does not affect accuracy and can be adjusted in 'Appearance'  See screen shot below
4) Once you copy the sketch, activate another sketch (on plane, face, or Mate connector) of your choosing and paste.  Use Transform if you want to move the sketch elements further.
5) This is done with several Feature Scripts - I use ExtrudeDir most often.  See screen shot below for 'Add custom feature'.

IsleofGough

Thank you, Bruce for your comments.
3) As far as I can tell, tessellation quality can only be assigned to a solid, not to a sketch. (See attachment). Maybe this is just a representation, but I am not sure this is how Onshape interprets the curve.
4) I can copy elements from one sketch to another and can rotate elements or transpose them within a sketch. I can also copy a sketch. But I am not seeing anyway to rotate or transpose an actual sketch. The only way to do this that I can ascertain is to create a solid with an extrusion and use the face for a new sketch.
5) That is helpful. Thanks!

john_mcclary

be assured, it is graphical.

if you are to ask Onshape to plot a point on that arc the output would be precisely what you would expect. The curve shows as a jagged edge because Onshape dose not waste processing time to show such a zoomed in sketch. This is not just Onshape, it is all CAD. AutoCAD at least gives you the option to enter a separate command to regenerate lines that will smooth arcs while zoomed in. But it really doesn't matter from a mathematical perspective, just an artistic one. And we are not artists.

tim_hess427

For your #4, you can't rotate a sketch, but you can change the sketch plane and then edit the sketch to make sure its still positioned where you want it on the new plane. 

Your options are to a) create a new plane and move the sketch to that plane or b) edit the existing plane's definition to re-orient it. 

tim_hess427

Also, for #1 - You can right-click on a part and change it's appearance (color and opacity), but there aren't photorealistic textures like Fusion360. 

and for #2 - No, there isn't a dedicated animation environment or tool. You can move things around in assemblies manually and animate a single mate (eg to rotate a linkage back and forth), but you can't do complex animations with "camera" controls and exploding assemblies and things like that. Also, there's no "recording" function either. 

IsleofGough

Regarding: "a) create a new plane and move the sketch to that plane or b) edit the existing plane's definition to re-orient it.", I don't see any way of creating a new sketch on a plane other than top/bottom, right/left, front/back without an existing face of a solid. Is there a way? 

Regarding "be assured, it is graphical.", that is good to know, particularly for trim operations. Illustrator does redraw at zoomed levels as does Houdini and Rhino and Fusion, at least better than Onshape. I haven't tried that in Solidworks yet.

So far, I find Onshape more straightforward and logical than other parametric CAD programs, so it is a pity it can't do photorealistic materials or animation. It does have advantages over the free version of Fusion in unlimited models, export to 3dm, and ability to use feet+inches in entering data and in drawings/dimensions.

tim_hess427

@IsleofGough - there is a plane tool that allows you to create new construction planes for sketches and things. 

Alternatively, you can define a sketch plane using an implicit mate connector that references existing geometry. 

IsleofGough

Defining a sketch plane using an implicit mate connector requires an existing part, right? The plane tool itself seems to have very limited options for defining a plane in space given a set of transforms and rotations. If I don't start with at least a line. What I was hoping for was the ability to define planes to do this sort of extrudes and rotations

tim_hess427

Implicit mate connectors just need some type of existing geometry. Once you place an implicit mate connector, you can also rotate and translate that connector as well. 

So, you can use a part or even simple sketch geometry. 

With a part like the ones you've shown, your best approach is probably like you suggested. Start with at least a lines and/or points, then use those to create the planes you need. 

steve_shubin

@IsleofGough said:

... defining a plane in space given a set of transforms and rotations.

Can do — 

Multi Mate Connector featurescript
https://cad.onshape.com/documents/5d8da63844bedebe5cff72b1/w/96a36142be717fc84a504e3f/e/11dcab8f665add80b9aced0a

1) The tool needs a mate connector to use as a reference. Takes 3 seconds to lay down your first mate connector.

Next you lay down your Multi Mate Connector using Delta X, Y & Z offsets and X, Y, and Z rotations

Finally, here is where a sketch drawn on the front plane is then changed to the plane of the multi mate connector

Multi Mate connector puts your connector a relative distance and rotation from whatever mate connector you choose

If you’re moving a sketch to a new location, then you may want to put the reference mate connector and the new Multi Mate connector before the sketch in the features list. And of course you could always do this after you’ve created your sketch. You could just re-order your features

konstantin_shiriazdanov

steve_shubin said:

1) The tool needs a mate connector to use as a reference. Takes 3 seconds to lay down your first mate connector.

The Multi mate connector actually doesn't neccesarily need existing MC, it creates new mate connector in the position difined by existing MC or inferred one with cooresponding transforms.

steve_shubin

@konstantin_shiriazdanov

Good thing I’ve got the author of that FeatureScript looking over my shoulder. Because I can’t even remember if I ever ever took time to look at that first field — LOL.

I’ve always just went with Default

So yeah I selected a couple of those and saw that I could get away without using a mate connector by using CENTROID and FACE.

There was no path in the example I used, so I didn’t have that option

I was able to select CENTROID and get the same exact result as when I used the mate connector

Now I’ve got reason to like the tool even more

Thanks Konstantin

👍