Align body centers to an axis, then rotate

[thepirate1]

Dear Community:  I am designing an optical system, so I place bodies centered on a beam, then rotate them in 3-space.  

What is the best way to do this? 

I found a similar question, said look at align command, I looked that up, said, "Snaps the selected object to a selected location on another object."  That's not waht I want. 

I am a newbie to F360(*).  I am on a mac.  

Let's break down the question: 

* How does one define an axis for alignment (that is not a physical object)? The axis changes every time I hit a mirror, of course. 

* How does one place the 3-D center of an object at a given location along the axis? 

* How does one rotate the body (e.g. a mirror)  appropriately in 3-space? 

* Please assume I am a complete newbie and idiot in your replies.  Beginner hints like "select this - it is highlighted when you are over it" are extremely useful. I can't even figure out placement at this point (How do you display the location and orientation of a body??)

Very greal thanks in advance. 

-TP

[Oceanconcepts]

OK, this should be relatively easy, with some organization. And as usual, there are probably multiple methods that would work, depending on the details of your design some may work better than others. 

Are your objects by any chance cylindrical? If so, you can create a construction axis through them- 

but first, make any distinct element in your system into a Component. Right click on a body in the browser, select Make Component from Body. The use of compost and basic structural elements is a principal key to happiness in Fusion.  

Activate the component you want first, then create the axis- that will keep the axis in the same component, so you can use it to align with other objects or axis. Activating components when you work on them is another key to happiness. You can align a component with another axis or a point as well as with another object.  You can go back to the root component (top node in the browser) the same way, by selecting its radio button. 

If you are wanting to position elements along a rail or path, I would start by defining that axis- if it’s a tube, then creating a center axis would be easy, if it’s some other shape you might need to define a point with a sketch first. But for ease, I would orient your linear path along one of the origin axis.

You can use the align tool

to position our elements along the main axis.

Any Component can be moved by selecting it in the browser with the right mouse button and selecting Move. I suggest a non-Apple mouse for CAD. The key to moving is understanding how to orient the Manipulator to get the direction of motion you want.   Select the Manipulator option, the Set pivot, and you can orient the manipulator to any face or object. The move tool allows precise moment in linear or angular settings, with numeric input if you want to rotate your mirror 22.5°.

I can’t do a whole Fusion course here, and this is just one possible path. You might, depending on your design, find it better to use Joints to set this up- a sliding joint, for instance. If you can post some images or files I’m sure you will get more suggestions.

[thepirate1]

Dear Oceans:  Thank you very much for your detailed reply.  your menu shots were very helpful.  It is a pleasure to hear from a fellow mac user. 

I learned a lot, could not find several of the commands you showed.  Thanks!   but ... Yes, still difficulties. 

* I learned from you how to use the Construction workspace to define an axis.  Its clear how to define an axis between two points.  However, I had a heckuva time positioning the points where I really wanted them.  It seems to me there should be a very simple way of simply locating these with X,Y,Z coords.  Couldn't find it.  Points are not listed in parameters (I can't understand why you can't just click on a body/component and get that info).  ----> Can you tell me how to locate a point (to make an axis with) by entering  X,Y,Z coords? 

--------Can you tell me how to enter these locations as formulae, with dependence on parameters? 

(You suggested using the origin - I can only use this once; every time I bounce off a mirror the beam changes directions to a new point in space.)

* I want to align the center of flat plane mirrors, which I model as boxes.  (I know cylinders are easier, but I need boxes.) How do I make my box-mirror into a component with the origin at the center?  

I was able to convert a body (a box) to a component.   I created a brand new box, and planned to move it to the workspace origin to get an origin at it's center, then convert it to a component.  Well, I got it well centered in two dimensions, but I could not get it centered properly in the third dimension (it was very thin and it was very hard to see if it was centered; I entered half it's thickness into the move pane, but it just didn't look right).  This would be very very easy if I could enter the X,Y,Z coords of the center point, or automatially select the center point as origin (a pretty obvious command!!!).  

-----------------> Can you tell me how to create a box with an origin for alignment at it's center (or the center of one face, also useful for a mirror). 

Hopefully if you or someone can point me to these two accomplishments, I would be able to get the rest of your suggestions. 

Thanks!!!

-Bruce

[Oceanconcepts]

There are lots of Mac users here, including many of the Fusion team. 

Access to commands in fusion is often workspace and context dependent- that is, if you are in the parametric, history mode, commands are different than in direct modeling. And there are the Sculpt, model, Patch, etc. workspaces. I’m assuming you are in model from what you say. Right clicking will bring up different menus if you are clicking on an object in the browser, in open space in the drawing, or with an object selected. There is a consistent logic to the interface, but it’s hard to just jump in without going through some of the learning materials and tutorials. 

Fusion doesn’t depend on a universal X-Y-Z coordinate system, each component has its own origin. If I understand correctly (and I might not) what you will need to do is to define your relationships on a sketch. You can set up user defined variables that can be edited and will update relationships, say distances between elements that are aligned along a sketch line. If you could post a simple version of what you need, any kind of picture or diagram, a suggestion might be easier.  Search the help or you tube videos for user defined parameters. 

“I want to align the center of flat plane mirrors, which I model as boxes.  (I know cylinders are easier, but I need boxes.) How do I make my box-mirror into a component with the origin at the center?  “

Create a new component. 

Activate it. 

Create a sketch that defines the rectangle you need.

Position a sketch point at the midpoint of the rectangle (using hints from the midpoint of each edge). 

Close sketch. 

Use the Extrude or the Push Pull tool to make the three dimensional box from the sketch.

-You will need to turn the sketch visibility back on after the extrude operation. 

Activate the root component.

You can now use the align tool (component option selected in the dialog box) to select the center sketch point to align to any other point in the drawing. 

Here is a screencast:

[thepirate1]

Dear Oceans: 

Thanks again for a detailed reply; the screencast is great.  I want to go over everything you suggested carefully, so I will need to get back to you tomorrow.  However, you asked for a sketch, so here is one generated in FreeCAD (attached).  The very thin boxes are mirrors; each causes a change in the direction of the beam, which we would implement as an axis line for each segment.  I want the mirrors to be centered on the beam, and of course oriented correctly, and eventually, the cameras (big boxes or cylinders which are only in the second image because they block everything) , to be centered on the beams. 

The exact feature I wanted to implement as dependent is the location of the mirror and its beam, dependent on the diameter of the big red camera.  If I change the diameter, I want the position of the beam to change in that one coordinate, such that the mirror and the beam are still centered on the middle of that big red camera cylinder. Hope this explains or at least illustrates. 

Thanks VERY much,

-TP

[TrippyLighting]

Therre are a several ways to create what you show in the screenshot. However, which one of these is the best way is difficulyt to determine without understanding what the end goal of your project is.

[TrippyLighting]

Based on the screenshots I created one way to do this.

The alignment and distance between the components is driven by a number of sketches.

The components are assembled to points/lines in these sketches.

Explore this and see if that would do what you need. Then we can continue the conversation.

I suggest, however that you also start watching some of the online tutorials, beause I thin a lot of your questions will be answered there.

[thepirate1]

Thank you very much for all your work and time in helping me - unfortunately I am not able to open the file you sent.  Can you tell me how to do this?  Searches on the web say this is a fusion file but requires special viewers. I must not be using the right procedure to open it in fusion? 

-TP

[TrippyLighting]

You need to upload this file to your Fusion 360  account using the big "Upload" button  in the dats panel in Fusion 360. Thsi is the panel to the left of the v3D viewport and browser. Once the file  shows up in the data panel you can open it.

I am pretty sure the upload prcess is covered somewhere in the video tutorials 😉

.f3d files are Fusion 360 archive files that are downloaded you your harddrive or wheever you want them. These are very handy for sharing single file projects here on the Forum by atttaching them to a post.

[thepirate1]

OK, I'm making progress understanding the suggestions here.

Just want you to know, Oceans,  that you cannot hear this screencast without super-duper amplified headphones. But it's very valuable!

Background: (Reprised) I want to orient a set of objects in space at specific parameterized locations. 

The suggestions from yourself and others seems to be use sketches to put points that will become local coord systems for each object, which you make into a component.  What is the "best practice" approach in this case:

a. sketch out lines to a location of each component, using the move command to locate the sketch planes

b. sketch out the lines using construction planes (construction>offset plane)

c.  [insert your best practice here]

Thanks, 

-TP

[TrippyLighting]

I don't think comnstruction planes can be moved using the move command.

Wht I did in my file was that I started creating a base sketche on two of the origin (construction) planes.

I then created other neede construcion planes using "Construct-> PLane through two edges.

I created all the components at the main origin and then assembled/joined them to points in the sketch. Look at the file I attached to my previous post and see if you can make sense of it. I can make a screencast perhaps o Friday. In general, however the video tutorials in the Fusein 360 learning resources should answer  lot of your question.

Also, there is not always a best pratice. Fusioen 360 offers many tools to get to the same end result in different ways. Sometimes it's simply preference. Other times it depends what the end goal is. You still have not told us that. 😉

[Oceanconcepts]

If you are in the direct modeling environment, not capturing design history, you can move a plane or sketch with the Move tool. But in the parametric environment, if you want to alter an offset plane, as an an example, you would need to find it in the timeline and edit the original instance. Sketches that have been used to construct elements essentially can't be moved, just edited. That is necessary to keep downstream dependencies intact. 

I second what Trippy says- there are often many ways to do something, and the appropriate strategy will depend on your goals or just on what tools you are most comfortable or familiar with. In your case, it might depend on what dimensions you want to be able to easily alter.  Doing CAD is a lot like working out a puzzle or a game, learning the tools is learning what moves you can make. 

[thepirate1]

Dear Trippy:

I think I am genereally getting this, and arriving at something similar.  

Here is what I did [attachment].   

You wrote, "Wht I did in my file was that I started creating a base sketche on two of the origin (construction) planes.

I then created other neede construcion planes using "Construct-> PLane through two edges." 

* If you are just doing a preliminary layout with drawn lines, how can you make use of two edges to make a sketch plane? 

* I am curious:  you did not seem to do any moves, at least, they did not show up in your history like mine did.  How did you orient the mirrors without moves?  

You wrote, "Other times it depends what the end goal is. You still have not told us that. ;-)"

Ultimate Purpose:  Select a CAD system that will let me conceptually lay out things at various levels of detail, occasionally for real production (mostly for illustration and my own better understanding/visualization).  I find that rendering instruments and things in 3-D is really useful, even if I won't really be manufacturing something direct from my work. 

Specific purpose of this drawing:  This is a multi-camera system for a telescope.  The light from the telescope comes through the ring (or mount plate).  What I called mirrors are really dichroics, that is, they pass or relfect only part of the spectrum, so e.g. the first dichroic will reflect all light except very blue, so the blue band camera on the other side takes the transmitted blue light, and the light reflected off that goes to the next dichroic, which selects the even more red light that goes to the big red cylinder camera.  The other camera takes the spectrum in between the two. I want to render this with cameras just as blocks, in 3-D, then show it around to get advice from more expert people. 

Next Step for me:  I need to look at documentation for assemble> rigid group; (perhaps that keeps construction planes and their bodies together, maybe as well as origins of the components and other stuff I'm not really aware of.)

Thanks,

-TP 

[thepirate1]

Dear Ron: 

Thanks for your comments here.  

There are documents and videos which refer to any action where you add constraints and enter values as parametric modeling.  There is also modify>change parameters where you can really enter changable paramters, which I cannot find documentation on (one of the videos for beginners shows this --- in one or two 1/64 s frames only.).  CAn you point me to documentation on how to do this? 

You spoke of the "direct modeling" environment.  Some video I found showed someone selecting create>base feature and it does not fully enter the history.  Is this what you are talking about? 

Thanks, 

-TP

@Oceanconcepts wrote:

If you are in the direct modeling environment, not capturing design history, you can move a plane or sketch with the Move tool. But in the parametric environment, if you want to alter an offset plane, as an an example, you would need to find it in the timeline and edit the original instance. Sketches that have been used to construct elements essentially can't be moved, just edited. That is necessary to keep downstream dependencies intact. 

I second what Trippy says- there are often many ways to do something, and the appropriate strategy will depend on your goals or just on what tools you are most comfortable or familiar with. In your case, it might depend on what dimensions you want to be able to easily alter.  Doing CAD is a lot like working out a puzzle or a game, learning the tools is learning what moves you can make. 

---

[Oceanconcepts]

Go to the Learning Home and search for Parametric- or any other subject you are looking for information on. Here is one video. 

http://fusion360.autodesk.com/learning/learning.html?caaskey=caas/CloudHelp/cloudhelp/ENU/Fusion-Get...

You can create a sketch generally as you want, then apply dimensions, user parameters, and constraints to get it precisely how you want. 

Create Base Feature puts you temporarily into a kind of direct modeling environment, but what I was referring to is the option in Fusion to not capture design history at all. In this environment some tools work more freely- I find it useful for working out a design in general terms. You enter it with a right mouse button on the root component. This option will delete any history you have, though. 

[HughesTooling]

Hi Trippy

Don't know if you've missed this or forgotten but you don't need to upload f3d files anymore, you can use New Design From File to open direct from your filing system.

Mark

[TrippyLighting]

Ha. I had seen the menu entry but not used it. Thanks for pointing that out!