Having trouble moving components into position precisely

[Anonymous]

I am trying to move a bracket into postion which will be used to join two tubes together of different diameters. Once I get them into position I will mirror and create a rigid group. 

The point to point move would work great if it could be restrained to a single axis. Further, it would be even better if I could set the pivot, then do a point to point move constrained along a single axis. I have a sketch which I should be able to utilize for moving into position but I cannot figure out how.

Is there some other way that does not involve creating additional geometry?

[joel.palioca]

Hello,

Have you tried leveraging joints to position your components?

Here is a quick link on it that is connected to a lot more information around leveraging joints.

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

Cheers,

[Anonymous]

Yes, I have tried using joints. The problem is that when I specify the joint origin there is no option to rotate it so that it is perpendicular to the cylinder. I can move it to the outside edge where it needs to be but cannot rotate it so make a proper joint with the other piece.

[TrippyLighting]

How are you going to connect the bracket to the tubes ?

[Anonymous]

Bolts of course. I know that I could create holes for said bolts first then create the joint. What I am looking for is a precise way of locating the parts without creating more geometry.

Being able to rotate the joint origin would solve the problem, so would being able to do a point to point move along a single axis. Is there another way?

[TrippyLighting]

Could you export your model as a .f3d and attachach it to the next post ?

Just trying to figure out if there may be a sketch in the bracket that can be utilized.

If not you may not have to create geometry but just a littel sketch in the bracket that you can reference off.

[joel.palioca]

Agreed as Trippy says a model can help us out.  I think we have some options here that we can investigate to help you through this, because there are multiple ways we can create joints.  We can leverage joints with the origins that show up normally, we can manually create our joint origins, or we can leverage the move/align command and use an as-built joint instead to lock down our degrees of freedom.

Hopefully with the model we can recommend a few different paths you can investigate.

Cheers,

[Anonymous]

Here's the file...

[Anonymous]

Using the move command and then an as-built joint was what I trying to do initially.

[TrippyLighting]

I'd aproach the structure of this design generally differntly and possibly much easier to handle.

As it is mainly a tubular structure I'd define the structure with a sektch with onlt the center axis off all the tubes.

Then I'd assemble all the tubes to that sketch.

[Anonymous]

Unless I misunderstand you, that is exactly what I have done.

[TrippyLighting]

Yes, I see what you mean assuming you a referencing the sketch in the "Tubing" assembly.

That does not go as far as I'd take it with the sketches.

Attached is a file with a bicycle frame, another structure made from tubes. Looks at the Frame and Bottom Bracket sketch and see  what it drives. You could do that similarly and make the overall size and structure of your assembly much more editable from a single sketch instead.

[Anonymous]

I think we are getting away from the problem here. I don't have a problem placing the tubing. I have a problem placing the brackets which go on the tubing because I cannot use a joint to locate them and I cannot use a move command with precision. I don't need the ability to alter the lengths or diameters of the tubing, or even the locations of the tubes. I don't see how the bcicyle frame is relevant to my issue.

What I wanted to know is how to move the bracket (front strut fixture) so that it ends up where it needs to be. I thought perhaps that I was missing something, maybe not. 

To say that I should apporach the design differently is all well and good but it does not answer the question of how to move something with precision. In SketchUp for instance I would only have to pick a point on the object, hold down the shift key then pick the point to move it to and I'd be done. Since the shift key was held it is constrained to move only on the active axis. I don't think it is unreasonable to expect Fusion 360 to be able to do something similar.

[TrippyLighting]

I had anticipated that youd say that but was hoping that I am able to take  shortcut 😉

I'll have to show it to you in a more complete fashion how I drive the bracket location from the same sketch.

[Anonymous]

Okay, well I don't want you to spend a lot of time on this. I know there are several other ways to get the part oriented as I need it to be.

Do you agree with me that being able to constrain the point to point move would be a useful thing? Or being able to rotate the joint origin along more than one axis? Either of those would make what I need to do a trivial thing.

[TrippyLighting]

I re-read your first post and lookig at the structure of your assembly I now get what you want to do. I believe attempting to move the parts into place with the move command or with Align will be difficult and is rather cumbersome if at all possible.

Whilst driving all the different tubes off of a single sketch, then creating componets from the extruded body you have backed yourself into a particular corner that is a little difficult to get out of with the move comand. The problem is that each individual component has it's own coordinate system/origin. As all of the tube bodies were not created at the original origin, after creating the components now all the circular tube profiles are offset form the origin and thus you cannot use that origin as a reference point for any of these tubes.

This woud be easy to do if you had used a single sketch for each of the tube profiles with the circles centered at the origin.

The way you first generated all the tube diameters and lengths and then re-used them in the assembly is really clever, so my recommendation would be to redo part of this by providing a sketch per tube profile. then you can use the origin as a reference point and it will make things much easier going forward.