Using Project command in assembly to add features to piece-part components

[paulQVFNN]

I am a new Fusion user and am able to create basic models (mostly formed sheet metal, machined carbon steel and STP files) and assembled them.   However, one problem I'm having is using the Project command to ADD features (i.e. through hole) to a piece-part that is assembled with other parts.  

In my current project, I have a basic 4-hole flange bearing casting that I want to bolt to a formed C-channel.  While in the assembly, in order to have the Project command available, I had to create a sketch on the sheel metal surface.  I can then project the flange's bolt pattern on to this sketch.  But this pattern does NOT show-up on the individual piece part file so I can actually create the hole pattern.  

In other words, I don't know how to add features to the piece-parts while in the Assembly.  I'm hoping there is a simple way to do this (while working with the assembly) as I often need to add features once I start the assembly process.

I have seen other 3D programs (i.e. Pro-E, Solidworks) where the user makes changes to piece-parts while in the assembly and these changes do actually change the piece-part.

Thanks!

[g-andresen]

Hi,

1. please show in a screencast what you want to achieve & what you do

2. please share the file, name the parts & what to do

file > export > save locally as f3d > append to the next post

günther

[wmhazzard]

In order to put holes in the sheet metal body, you just need to open a sketch on the sheet metal body either with the sheet metal component activated or with the top level active, and when in the sketch you can project the bearing bracket to the sketch. Then finish the sketch and extrude cut the holes.  

[paulQVFNN]

Thanks for your prompt reply.  A few questions:

When I create a sketch on the sheet metal face and project the hole pattern, I DO see the projected holes.  When I try to extrude them, I have an error msg that states something like "cannot extrude".  This may be due to the fact that the sketch has not been extruded so their is no "thickness" to extrude.  

And I guess this is where I am "lost".  The sketch is created on an existing sheet metal part to which I want to add the hole pattern.  

Your reply states "finish the sketch" and I'm not sure what you mean by this.   

Again, my goal is to project the pattern on to the existing sheet metal part AND have the pattern appear on piece-part model so I can create a drawing / dxf for manufacturing.  

Sorry for my ignorance on this!!

[wmhazzard]

At the top right corner of the sketch you will see "finish sketch"

If you can't figure it out, then attach an f3d file of your model to the next post. 

[paulQVFNN]

OK, I "finished" the sketch and push/pulled the holes.

I now see the holes on the sheet metal part in the ASSEMBLY as screenshot shows below.

This is similar orientation image of the piece-part and you can see the newly-made holes are not apparent.

How do I get the projected holes made in the Assembly to the piece-part so I can make an accurate flat pattern?

As I said in my first post, I'm a beginner.

I'm happy to send / share the f3d file, but what is the process to do this?

Thanks again.

[wmhazzard]

Once you have the projected holes in the finished sketch, select extrude and select the holes that you want and extrude cut the holes into the sheet metal part. 

[paulQVFNN]

I have done this and the images I sent in last posting show the holes through the sheet metal on the ASSEMBLED part.

This is similar image from other side of the sheet metal and you can see the extrusion operations in 5 places:

This is screenshot of the piece-part (similar position) which was inserted into the assembly. 

Again, you see there are NO extruded HOLES.

When I make a change (and save) on an individual part that is used in a Assembly, Fusion prompts me to update the Assembly to incorporate this change.  This makes sense to me as a change going "downstream" to the assembly.

However, are changes made to an part in the Assembly incorporated on the "individual part" file?  

Thanks for your help.

[laughingcreek]

it's possible we could answer better if we could at least see the browser tree i your pics.  even better would be to be able to see the uploaded files.

so a couple of questions just to check what your doing-

in your assembly file, is the part still "linked" (has the chain icon)?  are you doing " edit in place"?

or did you break the link to the part in the assembly?

did you insert the component, or derive it into the assembly?

[paulQVFNN]

Thanks for your comments.  The following is the screenshot you requested:

Looks like the "links" are in place.

I'm glad to upload the file, but have never done this.  Can you send a link with instructions?

[laughingcreek]

for assemblies with linked components, go to the file menu and export as a .f3z file to your hard drive.  then attach to post.

(fyi-usually files with un-linked components, exported as a .f3d file instead, are preferred.  But since the question is about the behavior of linked components you should use the .f3z in this case.)

[paulQVFNN]

Here you go on the exported file.

Thanks for your detailed instructions.

I am using the FREE version of Fusion 360 in case that makes a difference on functionality.

Just for my knowledge are changes made to inserted piece-parts in an assembly supposed to appear / take place on the actual piece-part (.f3d) file?

Really appreciate your help!

[davebYYPCU]

Short answer is to Edit in Place, the channel piece.  

You can extract the sketch and extrude the holes in the Assembly version, 

when finished save the Assembly, to transfer the edits to the channel.

open the channel file and you may need to get latest.

Give Alex time to read the files.

Might help....

[laughingcreek · Accepted solution]

You've got a few things going on here.

main thing is, if you want to edit a component, and for created sketches to go into the component, it's got to be activated.  for a local component that means turning on the radial dot next to the name.  for a linked component that means pressing the pencil for "edit in place". 

watch the screen cast.  you can see that your projected sketch went to the root component.  and you didn't cut any holes in the linked component, you just created 4 round new bodies, again in the root component.

but the bigger problem is your liberal use of "position captures" and "as built joints". and also the "move" command.  A design of this nature shouldn't have any position captures or moves  in the timeline. You can already see a symptom of these being in the time line when you go to the inserted component file.  the projected sketch is there, but it's shifted.  this is probably the result of one of those moves.  not sure.  it's not really worth trying to figure out, better to start over and use clean/robust modeling technique.

[paulQVFNN]

Thanks for your helpful comments and effort.  I was not of the edit-in-place feature and once I understood how this functions, I was able to make the edits.  I do need help on best practices for placing components within an assembly.  I don't like the Move command, but not sure how else insertion and placement could be done more quickly and efficiently.  

I'd appreciate any links to this type of training you could provide.

Thanks again.