Drawings that requier more than one page.

[RMPIII]

Hi,

   How do I add pages ( or sheets in Inventor) to a Fusion 360 drawing of an assembly.  I typicaly need to dimension elevations of the assembly, and then add an exploded view with BOM, and then drawings of the individule parts for inspection, and/or hand tooling.

Thank you,

Roland

[PhilProcarioJr · Accepted solution]

Currently you can't. You will have to do multiple drawings. It's on the roadmap though.

The roadmap for 2016 says:

"

Drawings

A continual focus on drawings to round out the tool necessary to create fabrication drawings this includes but is not limited to :

• Text Formatting
• Annotation types like surface texture and weld symbols
• Finer level of control on annotation formatting
• Additional view types and display of threads
• Spline leaders and title block visibility controls for Patent Drawings
• Multiple Sheets
• "

http://forums.autodesk.com/t5/fusion-360-product-roadmap/a-preview-of-where-fusion-360-is-headed-as-...

[dthoffman225]

I was looking for the same option, but found the same answer.  I know that we can make components inside of an assembly, but how do we document all of the custom made components?  Will I have to export them out of the assembly to draw them individually?  Will a link to that part then be created inside my assembly if that is the answer?  That brings the Fusion 360 concept back to a top down design similar to any other CAD program.  What I love about 360 is that I do not have to have a bunch of links to project specific components. If it were just about the design but not the manufacture of the parts, then 360 rocks, but I want to build what I create.

David

[PhilProcarioJr]

@dthoffman225

I agree with what you say, but you got to understand drawings in Fusion are still very new and are being worked on. They are aware of the shortcomings and I'm sure over time they will develop them into something very useful for us all. In the meantime we just have to deal with what we have or use a different package. 

[andrew.de.leon]

Hi David,

Unfortunately, we can't create multiple sheets within a single drawing yet. We do have it on the roadmap, but at this stage we don't have a release date.

To answer your "...how do we document all of the custom made components?  Will I have to export them out of the assembly to draw them individually?" question, no, you don't have to export each component out of the assembly before creating drawings. When creating a drawing, you can select the full assembly (default) or one or more individual compoenents. Regardless of what you select, each drawing creates a link back to the model. If you create a drawing of the full assembly, the drawing creates a link back to the model. Llikewise, if you create a drawing of a single component within the assembly, the drawing creates a link back to the same model. Although they are seperate drawings (within the Data Panel), each drawing is linked to the model so that changes made to the model update all drawings. These links can are then displayed in the Data Panel.

To create a drawing of the full assembly, launch the New Drawing from Design command and in the CREATE DRAWING dialog, make sure the Full Assembly checkbox is selected.

To create a drawing of a single component, launch the New Drawing from Design command and in the CREATE DRAWING dialog, unselect the Full Assembly checkbox and select the component you want to create a drawing of by selecting it within the model itself. BTW, you can select more than 1 component if needed.

To track all of these links, open the Data Panel and click on the information "i" button in the lower right corner of the model. This will open the detail panel for the model and list all links to drawings as well as parent models.

I hope this helps.

Thanks,

Andrew

15" Retina MacBook Pro (Late 2013), OS X El Capitan (10.11.3), in Sydney Australia

[dthoffman225]

Thank you, I must say, I am very impressed with the technical assistance I am getting while I learn my way thru this software.  I will try this on my current project.

[RMPIII]

Dear PhilProcarioJr,

Thank you for your help.  This answered my question, and keeps me from banging my head against the wall.

Thank you again,

Roland

[Anonymous]

Hi,

Just a comment on this post. I have just tried the solution given, and it does not work.

I get the complete assembly in the drawing, no matter what I do.

Regards,

Brett

[Anonymous]

Hi,

I just re-read my post, and I think I was a bit skimpy on the details of my problem.

Part of the question was - How to do a drawing of a individual component or body in an assembly (or words to that effect).

I tried the suggestion given,

     To get a drawing with only 1 component of an assembly

     Unselect the tick box next to "Full Assembly"

     Click on the actual component in the design

     Click on "ok"

It does not work.

Regards,

Brett

[krithika.sundararajan]

Hi Brett,

Is it possible you are trying to select a body (and not a component)? If this the case, selecting the body would still selet the entire model. Is this what you are seeing?

To be sure, you could try to do this from the browser tree. You could select one or more components from the browser tree > right click > choose Create New Drawing.

The Create New Drawing option will not appear for bodies. In this case, the body can be placed in a component by selecting it in the browser tree and choosing 'Create Components from Bodies' from the right click menu.

Let us know if this works for you.

Thanks,

Krithika

[Anonymous]

Hi Krithika,

Ok, question, can I create and edit a body inside a component?

Regards,

Brett

[krithika.sundararajan]

Hi Brett,

I'm no expert with modeling but let me try to answer that.

In Fusion, by default, bodies are created under the root node. They can be converted into components by right click > 'Create Components from Bodies'.

Empty components can be added under the root or under existing component by selecting it and choosing 'New Component' from the right click menu:

To move a body to an existing component, simply drag the body (from the browser tree) and drop into the component.

Also, with most/all Create body dialogs, there is an option to create a new component as well.

To make sure any newly created bodies always fall into a specific component only, you can right click the component in the browser tree and select 'Activate'. When done, we can Activate the root node again.

Did that help answer your question?

Thanks,

Krithika

[MattPerez314]

Krithika said it but to clarify you can have multiple bodies in a compoment. You can create and modify bodies in a component. One great benefit to this is when you activate a component the timeline only shows features associated with it.

If you know your file will have components its a good idea to start with empty components. Be careful with the new "create compoment" button on assemble. By default it will activate the component and if you keep creating you will be nesting them essentially creating sub assemblies.

[Anonymous]

Ok, Thank you.



Regards,



Brett Clausen

BMX Engineering cc

011 882-1575

brett@bmxengineering.co.za

[yebyps]

Making a drawing file of an assembly with several pages, each detailing a component or set of components.

This drove me crazy for at least a week, after following advice on forums to go via animations to achieve this, but it's not necessary.

• Create a drawing From Design, but untick the Full Assembly option.
• In the option to Select Components, select all the components in the assembly. You can do this graphically or by selecting the top level assembly item in the browser. Select your options for Creating New, template, standard, units, and sheet size then OK.
• By default, you can click on the initial position of the base drawing, which involves the full assembly, and construct the projected views you want. Normally you'd want to start off with the full assembly anyway.
• Then click on the Plus sign on the bottom of the screen left to create another page.
• Add another base view. This time, in the browser, you can switch off (click, shift-click, right-click, Show/Hide) all components you don't want to show and end up with a single component. Then dimension, view etc. for that component. 
• Keep adding sheets and singling out components to your heart's content.
• Tip. Right now you can't add sketched lines for emphasis/dimensioning in a drawing. But you can go back to the component in the model and add a sketch which has the lines or other sketch elements you want to dimension in the drawing (like angles for circular patterns). You have complete control over which sketches are showing in the drawing browser. Construction lines don't show, only projected and solid lines. I guess you could also have a sketch including text but I haven't tried that.