How to Insert Another Component Into A Drawing

[BASF_Ace]

Hello Everyone,

I've been spending the past week trying to familiarise myself with Fusion 360. I'm coming from SolidWorks so a lot of things are unintuitive to me. 

I'm having a hard time creating drawings.

Firstly I have an assembly made up of 6 distinct components.

I want to make 2d drawings of each component all on the same sheet, but I can not seem to do so.

Secondly, I would like to make drawings composed of multiple sheets. Is this even possible in Fusion 360?

Thirdly, drawing in Fusion 360 seems pretty NERFed when compared to other CAD software. I realis that this is a new feature, but are there plans to expand it in the future?

[scott.price]

Thanks for the note,

Unfortunately a drawing can only contain one part or assembly reference at this point - this is something we will be improving but it is a large undertaking and we're prioritizing it against other features and areas drawings is lacking. Likewise for multisheet drawings.

Drawings is actively being worked on and you should be seeing incremental improvements and new capabilities coming online quite regularly. Were there any other specific issues you were having that were blocking your drawing creation?

Best,

Scott

[BASF_Ace]

Actually there was one bug I noticed.

When trying to create a new drawing from inside the modelling environment a new tab is opened with the drawing in it. (It goes straight to the base view)

Anyways I wouldnt be able to place the view on the sheet at this point. It would appear as if the mouse was stuck behind the dialog box. This happened more than once, but it went away after I restarted Fusion. I have not run into the bug again.

[0502880]

Hi @scott.price,

I haven't tracked the drawings roadmap well; is there some plans when it could be possible to add several (sub)components to same drawing sheet? Because it would be in many cases nessecary and much more informative to get an assembly constructed of 2-4 parts and it's individual subcomponents presented/dimensioned separately in the same drawnig sheet.

Another question concerns the possibility to draw/sketch "helplines" directly to drawings, now it's sometimes nearly impossible to show certain angles/dimensions in the drawings.

-Juha

[0502880]

@scott.price, sorry, just noticed that in current version it's already possible to add several components to same sheet! Good! Haven't made any drawings for a while...

Still the question about "help" lines in the drawings is still valid...

-Juha

[mishrani]

Hi @0502880,

As of now it is not possible to draw/sketch lines directly to drawing. But recently we released a feature to expose 3D sketches in drawing environment.

If you have a 3D sketch that can be used as reference/help line, you can enable it in drawing environment.

Here is the help link for Sketch visibility :

http://help.autodesk.com/view/fusion360/ENU/?guid=GUID-F8A74139-8058-43D1-B17B-5451149301AD

Hope it helps!

[0502880]

Hi @mishrani,

thank's for your answer! Sure the sketch visibility helps in many cases, but with some tricky components the "helplines" could sometimes help.

[Anonymous]

ok... 4 YEARS later and this has still not been addressed?

[jhackney1972]

in my Screencast, I show you how to place multiple components on one sheet of a drawing and on multiple sheets.  Please note as I do it, the Create Drawing dialog box, this is where you specify which drawing and which sheet in that drawing you want to place the component drawing in.  If I misunderstood your question please let me know.

Your last statement that Fusion 360 drawing environment is Nerfed, as you put it, compared to other CAD applications, I will remind you that Fusion 360 is a FREE package for many and for those on subscription an small price compared to those OTHER CAD applications I am sure I could name.  It will improve but for right now, just learn to use it to its maximum efficiency.

[laughingcreek]

@Anonymous -which aspect are you referring to as not being addressed?

[andrew.de.leon]

Hi @Anonymous,

Just curious what you’re trying to achieve here. If you’re trying to place drawing views of components from the same assembly into the same drawing sheet or even different sheets in the same drawing, this has been possible for about 3 years now (maybe slightly longer). But if you’re trying to place drawing views of multiple different components into the same drawing sheet, this is still a limitation.

If its the first, open the model containing your assembly and the drawing you want to add to. Then, in the model select the component you want to add to the drawing within the browser, right mouse click and select Create Drawing. When the dialog appears, change the Drawing property from Create New to the existing drawing and if required select an existing sheet or new sheet and click OK. Fusion will switch to the drawing and you’ll see a base view of your component attached to your cursor ready for placement. Place the view and you’re done.

The other alternative is from within the drawing, launch the Base View command which will preview the entire assembly. Place the drawing view. Then, select the component in the browser, right mouse click and select Suppress All Except Selected. This will suppress all but the selected component.

Hope this helps but if I’ve missing anything let me know.

Cheers, Andrew

[Anonymous]

It's the latter case.  Don't worry about it.

[ersin.bilgin]

thank you my firend problem solved 🙂

[scott.horton7KAQV]

John, thank you for that video.  Just what I needed.

[terriHEKCJ]

Hello,

In response to @andrew.de.leon :
"But if you’re trying to place drawing views of multiple different components into the same drawing sheet, this is still a limitation."

Has this been resolved? I have two almost-identical pieces in two separate files. I'd like to combine them on one drawing. Coming from SolidWorks, I would normally create one file and produce two configurations. From what I'm seeing online, Fusion doesn't support a feature like this yet.

So, basically, is there a way to put two different parts (not assembled) onto one drawing?

[g-andresen]

Hi,

1. create a new design, save it and insert the desired designs from the datapanel.
2. create several drawings from the (new) design on the same worksheet and activate the desired parts.

günther

[terriHEKCJ]

Thanks, @g-andresen 

This work around worked for now. Was hoping not to have to create another new file but hopefully Fusion can figure something out in the future.