Joints - Using reference geometry (planes, axes and points)

[Anonymous]

Hi,

First off - I'm coming from  Solidworks / ProE background which is definitely affecting my expectations...

I have a part imported as an IGES file.  I'm designing an enclosure and associated componentes around this IGES part and need to use various geometries of the IGES file as reference for engineering features on the enclosure.  I would prefer to place the IGES file into the design first and fix it in a desired location before building the other geometries/components around it.  I could of course work differently but I'm evaluating Fusion 360 and trying to understand the various workflows....

My ultimate assembly is bilaterally symmetrical.  I would like the IGES file to be located in the center.  Given that the IGES parts default planes are not appropriately located, I would normally create reference geometry in the IGES part using whatever means required so that I had planes bisecting the IGES file or an origin at its center.  I would then use that reference geometry to create "Joints" (mates in Solidworks) to align the IGES file with my assembly's default planes.

It seems that planes and axes are not selectable during the joint process.  What's the appropriate workflow for Fusion 360 given what I'm trying to do?

Thanks for reading the long-winded description!

[kgrunawalt]

The joint command uses two "joint origins" to create a joint. It can define them on-the-fly by selecting geometry, or you can create them ahead of time using the joint origin command which has more options. A joint origin is essentially a UCS (user defined coordinate system).

Both the joint and joint origin commands can use construction geometry, but you need to use a workpoint/construction point in addition to planes or axes. The joint origin requires a point at least. This point should be in the component that will be joined (very important!). You might need to activate the component before adding the point.

The joint origin command (or the on-the-fly joint origin definition via the joint command) will infer orientations from the point geometry if possible or use the origin axes of the component owning the point. If you predefine the joint origin, you will have more options to customize the individual joint origin's axes by selecting geometry including construction axes.

There are a number of ways to define a construction point.

Hope that helps!

Katrin

[kgrunawalt · Accepted solution]

BTW, you can also use sketch points to define joint origin locations. If you need to put a point at a location that is dimensioned from an existing point, you can create a sketch in the component and use dimensions to locate the point in the sketch plane.

[Anonymous]

Thanks for your help... It's hard to shake off the Solidworks / ProE logic.  I'm enjoying the software but I'm a little frustrated - I can't seem to find a complete manual / user guide.  It's making the pace of learning much slower than I would like. Any advice that doesn't involve videos?

[kgrunawalt]

Good point about the help. We mostly have video-based help which is great in some ways but something you can browse as a reference. I'll ask if we have something or plan to that is more of a reference.

[Anonymous]

I'm having very similary difficulties.  There are so many things that seem like they shouold work or there shuold be a way to do something, but it doesn't seem to work in Fusion 360 and there are no comprehensive manuals.

I'm sorry if this is a bit ranty, but this was an issue I was hoping to get clarity on, but like the original poster I am not finding this very usable coming from Solidworks.

-I have a model I created in Fusion 360, then placed it into another model intending to make it an assembly, but I can't do basic things like select features of the first part to create joints or relationships.  I can't hide or show geometry because "it's read-only", but it doesn't matter because even when I have geometry I can't use it.

-In a sketch, I can't drag a point onto an edge and generate an automatic relationship.  I have to explicitly create each relationship.  

-There are apparently no hotkeys or ways to set shortcuts.

[Anonymous]

Hi, I've heard it can be somewhat different to wrap one's head around after coming from a different software.  A search returned some apparently valuable material. 

On this youtube page, there is a section with multiple videos called "top 10 tips for solidworks users" or something to that effect, that looks valuable.  There are also lots of other tremendously valuable tutorial videos on that channel.

https://www.youtube.com/user/AutodeskFusion360

Also here's some other relevant materials:

https://www.youtube.com/watch?v=6tmAG7Hw1g4

the above came from another thread, which has some additional information: http://forums.autodesk.com/t5/design-and-documentation/best-practice-for-top-down-assembly-design/td...

http://forums.autodesk.com/t5/design-differently/from-solidworks-to-fusion-360-time-dependent-mates-...

http://forums.autodesk.com/t5/design-differently/from-solidworks-to-fusion-360-my-first-2-weeks/ba-p...

http://forums.autodesk.com/t5/post-your-tips-and-tutorials/fusion-360-to-solidworks-table/m-p/574840...

http://knowledge.autodesk.com/support/fusion-360/learn-explore/caas/CloudHelp/cloudhelp/ENU/Fusion-F...

[TrippyLighting]

First of all welcome to the forum!

In the upper right corner is a hel or question mark button that will lead ot the written documentaiton that will get you started.

As a former Solid Works user myself (12 Years) I'd say this section will be most useful to start with because the concept between components and bodies is not that obvoious and mostly hidden in SW.:

http://fusion360.autodesk.com/learning/learning.html?guid=GUID-6F85C4E9-3361-4866-AD16-F37F37037A7D

In general the "Build Assemblies" Section in the Fuaion 360 Learning ressources will be interesting. In SW, when you mate parts you basically are creadig geometric constraints such as "this concentric to that" etc. Fusion 60 works with the concept of Joints which is quite different.

Also, once you understand that most of your stuff should end up in a component don,t select stuff in the viewport and use the move command on it as it is likely not what you want to do.

[patrick.miller]

Hey AJameson56,

Totally agree with the reponses above. A few things to add:

What you describe with joints does not sound expected. A few things to consider: Does the design contain components or only bodies? Is the inserted component grounded (thumb tack in the browser)?

Bodies and Components: http://fusion360.autodesk.com/learning/learning.html?guid=GUID-E37B0456-A867-429F-BF69-6A4626DD31E7

Joints: http://fusion360.autodesk.com/learning/learning.html?guid=GUID-6A781281-1D14-4C95-BAFD-8489E500D3D2

Kevin Schneider's joint brain dump: http://forums.autodesk.com/t5/design-and-documentation/let-s-talk-about-joints/td-p/5493427

If I'm reading the sketch question correctly, you'd like to drag the end point of a line onto the edge of a 3D box/geometry. You are correct that you need to explicitly create the constraint or project the edge in first. I'd suggest adding this to the IdeaStation to get it considered for a future release. I'll also ping the sketch UX designer to see her thoughts.

Very few hotkeys today but we are adding hotkeys in the Sept update. For Sept, we are adding what were determined to be common hotkeys. Its planned to add a customization UI in a later release.

Hopefully this helps. Happy modeling!

[Anonymous]

Thanks for the several responses.  Some of this is learning curve, and I'm encouraged by the content y'all have pointed to, to keep coming up the learning curve.  There are several things I've discovered incidentally that are making the transition from SW easier.  

Some is also lack of features, and I'm happy to see some progress by looking at comments about upcoming features in IdeaStation.  I'll continue to add a few things that would make the SW easier for me to use.

For context, I'm in a startup and am trying to save money by not getting SW, at least yet.  I've committed to giving F360 a good try, and I'm more optimistic now than I was earlier in the week.  I've worked in the medical device R&D field using SW for the past 7 years, and used SW in school before that.