Reorient axes?

[keithd]

I have a complex assembly. Several components, sketches, joints etc.

Somehow it got drawn at 45º to XY plane sitting on the XZ (base) plane. I want it rotated to remove the 45º and fthen lipped so so it sits on the XY (base) plane with Z up.

Moving all the components to the correct orientation would be a terrible job. Leaving it wrongly oriented is annoying and screws up other stuff, like creating 2D drawings and CAM.

Is there any way to simply reorient the axes to the assembly. I've tried everything I can think of.

--

Keith

[James.Youmatz]

Hi @keithd,

I don't believe you can reorient the axes, but I'll dig a little bit deeper to check it out. Depending on how complex your model is you may want to check out the align command in the Modify menu. You should be able to select your bodies and align them to the Origin or Origin Planes. If you want, you can share the model with me (james.youmatz@autodesk.com) and I can take a peek and hopefully create a screencast detailing how I would go about reorienting your model. Try the align command first and let me know how it goes!

Thanks,

[HughesTooling]

Although this will not help you with drawings you don't need to worry about orientation for the CAM work space, you can orientate the setup to your model easily.

Mark

[keithd]

Hi James, Okay, I just looked at align. But I can’t imagine what it even means in this situation. As I said, the assembly has many pieces. And I need to reorient the whole assembly in space. Align, as I understand it, allows you to align two entities. First, there is no entity that I could align it too. I want to reorient it in space, i.e., to nothingness. Conceptually, I guess I could create a temporary entity to align to. But in thinking about that I can’t see what to actually do. What entity would I create? Where would I place it? (I want the origin to remain exactly where it is relative to the assembly.) If I select all the pieces of the assembly, then wouldn’t it try to align each piece with the temporary entity? That would explode the assembly. Lets say the temporary entity I create is a, well I can’t even think of a suitable one, but lets just say a box. What would it mean to “align” the assembly or all the oddball shaped components in the assembly to a box? I actually just went an tried it, but the Align command wouldn’t even let me select meaningful things to align. Anyway, I would be glad to share the model with you, but I don’t know how to do that. I tried File:Share, but it would only let me share with the whole world. It wouldn’t let me enable download or require a password. I couldn’t see any way to share it with just you. It’s not something I’m trying to hide from the world, but it seems like overkill. (I’m trying to learn to love Fusion 360, but the Cloud aspect of it is definitely NOT something I care about or will ever want to learn to love.) Thanks for the response. — Keith > Hi @keithd , > > > I don't believe you can reorient the axes, but I'll dig a little bit deeper to check it out. Depending on how complex your model is you may want to check out the align command in the Modfiy menu. You should be able to select your bodies and align them to the Origin or Origin Planes. If you want, you can share the model with me (james.youmatz@autodesk.com ) and I can take a peek and hopefully create a screencast detailing how I would go about reorienting your model. Try the align command first and let me know how it goes! >

[HughesTooling]

You might be able to insert the whole design into a new design and orientate the part when it inserts how you want it then break the link to the original file. Again this might not help with drawings as each component has it's own origin and origination.

Mark.

[James.Youmatz]

Hi @keithd,

So my suggestion of align would be difficult with the many components you are working with, but I can check. @HughesTooling had some great ideas too! I'm sorry to hear the Share Public Link button wasn't working 😞 If you go to https://myhub.autodesk360.com/ and then access the file you are working on you should see a sideways carrot (<) with three dots. This is the Share Public Link button. I know you said you're not a cloud guy, so I'm sorry for having to send you to the cloud! Once you do that, if you could just share it with me that'd be great. If not, just download the file as a .f3z file (from the A360 website not Fusion) and send it to my email if you need to. Try the share public link button first though.

In regards to the align command questions you had - I guess I am a little bit confused. I thought you said you it was 45 degrees rotated about the origin? You can align components (whether it be their origin or a face, edge, vertex, etc.) to the global origin (the point) or the planes (XY,XZ, YZ). Like I said, without seeing the model it is hard to speculate what the best practice would be in this situation, but I will take a look as soon as I get it. As you mentioned though, since this has a lot of parts, it may be hard to perform it that way but I will take a peek. Perhaps other users have some suggestions as well and would be willing to chime in.

Thanks,

[Oceanconcepts]

This kind of thing is something I have had to deal with, and I’ve often wished for the option to reset the origin in a component. I have learned to pay attention to the origin when I create a new component. 

First, as to what to align with, one idea would be to create an offset construction plane using one of the origin planes. Use the Align Components option and the geometry you select on a component will snap to the plane. 

As to how to align the whole assembly, here is something to try: 

1. If you have a complex assembly, make sure it is encased a single component- that is, put all of your assembly, everything you need to align, into a single master component. You may need to make a new component and move all the others inside it by dragging in the browser. Or you may already have your design organized this way. 
2. Turn that component into a Rigid Group- right click on the master component in the browser to access this command. 
3. You should then be able to use the align tool, select some appropriate geometry on the component, and align that with the plane you select, while preserving the design structure. 

I’ve only tried this with a simple set of components, so I don’t know if there are hidden issues with some sorts of geometry. But it should work. 

[keithd]

I went to the Share button on the Web site as you suggested and it gave me this link. http://a360.co/1NV5api The button is on to "Allow viewers to download to their computer." Is this what you mean by “share it with me?” Seems like I’m sharing with everyone, not just you. That’s okay, but it seems odd. I would have thought there was a way for me to share this file with James Youmatz. — Keith > > So my suggestion of align would be difficult with the many components you are working with, but I can check. @HughesTooling had some great ideas too! I'm sorry to hear the Share Public Link button wasn't working If you go to https://myhub.autodesk360.com/and then access the file you are working on you should see a sideways carrot (<) with three dots. This is the Share Public Link button. I know you said you're not a cloud guy, so I'm sorry for having to send you to the cloud! Once you do that, if you could just share it with me that'd be great. If not, just download the file as a .f3z file (from the A360 website not Fusion) and send it to my email if you need to. Try the share public link button first though. > > > In regards to the align command questions you had - I guess I am a little bit confused. I thought you said you it was 45 degrees rotated about the origin? You can align components (whether it be their origin or a face, edge, vertex, etc.) to the global origin (the point) or the planes (XY,XZ, YZ). Like I said, without seeing the model it is hard to speculate what the best practice would be in this situation, but I will take a look as soon as I get it. As you mentioned though, since this has a lot of parts, it may be hard to perform it that way but I will take a peek. Perhaps other users have some suggestions as well and would be willing to chime in. > > > Thanks, >

[keithd]

That sounds like it might work, but how do I "insert" the design into a new one?

I looked for a way to do this but couldn't find it. I tried several approaches but no luck.

How the heck do you guys know all these tricks? Is there a Fusion 360 manual somewhere that I'm missing? I've watched most all of tutorials, but I don't see in them many of these kinds of tricks or many of the other operations I see people using on YouTube videos (e.g. from NYC CNC).

Thanks.

--

Keith

---

@HughesTooling wrote:

You might be able to insert the whole design into a new design and orientate the part when it inserts how you want it then break the link to the original file. Again this might not help with drawings as each component has it's own origin and origination.

Mark.

---

[keithd]

The design I'm working on was my first Fusion 360 design when Fusion was in early beta. Things like drawings and CAM didn't exist so I didn't realize it was going to be important. Or that reorienting axes wouldn't be possible. Other design packages I've used, like SketchUp, make reorienting axes trivial. Now I know to take care. But even if you take care at the start, a design could easily evolve in a way that might cause you to want to reorient the axes. 

Per your suggestion, I tried aligning components with a construction plane. No luck. It keeps telling me "No alignment suggested by geometry could be found."

My entire assembly is already encased in a single componet. I tried turning it into a rigid group. But aligning it to anything doesn't seem to work. It keeps saying "No alignment suggested by geometry could be found."

I'm guessing there are too many oddball shaped components or the working joints between components is preventing alignment from working.

--

Keith

---

@Oceanconcepts wrote:

This kind of thing is something I have had to deal with, and I’ve often wished for the option to reset the origin in a component. I have learned to pay attention to the origin when I create a new component. 

First, as to what to align with, one idea would be to create an offset construction plane using one of the origin planes. Use the Align Components option and the geometry you select on a component will snap to the plane. 

As to how to align the whole assembly, here is something to try: 

1. If you have a complex assembly, make sure it is encased a single component- that is, put all of your assembly, everything you need to align, into a single master component. You may need to make a new component and move all the others inside it by dragging in the browser. Or you may already have your design organized this way. 
2. Turn that component into a Rigid Group- right click on the master component in the browser to access this command. 
3. You should then be able to use the align tool, select some appropriate geometry on the component, and align that with the plane you select, while preserving the design structure. 

I’ve only tried this with a simple set of components, so I don’t know if there are hidden issues with some sorts of geometry. But it should work. 

---

[Oceanconcepts · Accepted solution]

I downloaded your file, and I was not able to get my suggestion to work either- until I ungrounded the Base component. That’s the key. I’ll note that it was not necessary to turn the container component into a rigid group. I was thinking previously that you had the entire design on an undesired orientation. I now understand that some of the components were created with an origin coplanar with the XY plane, but rotated 45° around the Z axis.

So your issue is not having internal origin consistency within the design? Each part in Fusion has its own origin, rather than like some other programs creating everything from reference to a drawing origin. I’d ask what problems you see with these different origins? It shouldn’t make any difference for drawings or CAM. I’ve never found any way to change the origin of a component once it was created. The only irritation I have found is that when you select Move, the default orientation of the tool may not be what is desired- but if you select the manipulator, you can easily re-orient the move tool along any geometry.

As to your insert question, any design that appears in your data panel can be right clicked on, this will give you the option to Insert Into Current Design. You can also select components in your design and chose to Save Copy As- that will put the component into your data panel for use in other designs.

If you want to reorient in space the entire assembly, Mark’s suggestion will also work- open a new design, save, then right click in the data panel and chose Insert Into Current Design. You then have the option to move the entire design freely.

A lot of confusion is around understanding how bodies and components work in Fusion- that really is key. Any element of your design that is a distinct part of the assembly should be defined as a component. Activate components when working on them so construction geometry ends up with the component rather than in the root level. You can nest components to create sub-assemblies. Many Fusion actions can only be taken on Components. It’s actually pretty powerful as a tool.

You are correct that the documentation on Fusion is a bit thin, particularly with respect to tool and command reference. It’s a rapidly evolving program. I’ve learned to always experiment with right clicking in the drawing and in the browser to view the different menus. There is a logic to the program, and it does get easier as you work with it- hang in there and I think you will find the forum here helpful.

[robduarte]

I know that this is an old topic, but to answer the question of why this matters... The animation workspace. If you want to use the auto-explode feature, the axes for all of your components had better be oriented in the same direction or the exploded view it produces will look like a real-life explosion with parts going in all directions. It would be nice if the axes could just be reassigned (ie: "green should be red" by right clicking on the axis line and changing it).