moving sketch/body/component to new file?

[jskinner58]

Have a project (not completely sure that's the right term...) with multiple components.  The components are basically sheets of material with slightly different outlines.  I want to place those outlines side by side in another file so they can be cut from a larger sheet.  Looking at the existing design I don't find sketches that match the outlines - I think I must have extruded to the side to get the overall size as the interior shape (a cutout) is key and the outside just had to be big enough to include the shape and fasteners to hold the sheets together.  Wondering the best way to proceed.  I think I could project a sketch for the overall outline of each component within the component which seems like it would be useful going forward.  Then copy the sketch.  Or I could copy the component and make any sketches needed in the larger plate file.  CAM of the larger plate would be water jet to rough cut the outline of the plates plus the interior cutout and fastener holes.  The plates will then have some final milling - fastener head recesses, etc. 

Second question is if I make a new main model what things could I do differently to make this easier?

[jhackney1972]

Please attach your Fusion 360 model.  Open the file in Fusion 360, select File then Export and save to your hard drive.  Attach it to a reply post.  You should also probably indicate the entities you want to move/copy. 

[jeff_strater]

I'm a little confused.  Your title and your description don't seem to match.  Your title seems like it is a question about how to take a local component and save it to a new design.  For that, just right click on the local component, and choose "Save Copy As".  That will create a new design with just the features for that component.  However...  If that component contains references to things outside that component, the resulting design may not be ideal.

However, your description seems more like some basic workflow questions that probably need a bit more explanation, and as @jhackney1972 says, your current design.  Depending on how much you have put into this, it might be better, and even easier, to start from scratch.  I often do that with designs.  The first iteration is for learning, and the second time around, I can do things much more cleanly, and efficiently.  So, don't discount just starting over.

[jskinner58]

I made a simplified file that is similar.  From the assembly I want to take the individual components and place them in another file for cutting them all out of a larger piece of 0.5" thick steel with water jet.  This will probably be a dxf file output.  I see how to move the components to another file.  But the layout details (a sketch) are part of the assembly so they don't carry over.  I want to make some adjustments to the outlines - mainly offsets to allow for the kerf of the cut and leave some additional material for finish milling.  Looks like I will need to project a sketches from the components?

[laughingcreek]

I think what you want is derive.  that will allow you to bring just sketches and bodies you want into another model.

[jhackney1972 · Accepted solution]

The video will outline a "long winded" process of copying the original sketch to each of the components so when you Copy/Paste New to a new file, you will have both the component and the related sketch to edit.  I copied to the same new file but you could use separate files for each. Model I used is attached.

[jhackney1972]

The OP had this line in his last post " I want to make some adjustments to the outlines - mainly offsets to allow for the kerf of the cut and leave some additional material for finish milling."

Your suggestion is a good one but I am wondering how he will be able to edit the sketch, for each component, and have the component update?  If there is a way to use the Derive and still use the sketch to modify the component dimensions, would you create a short video of the process, I really need to know it!

[jskinner58]

Thanks John!  Very helpful.  I realized after I posted my model that in my more complex file I did a sketch on a side plane and extruded for the size of the plates and then cut them with the top sketch for the outlines.  So I don't have a sketch of the outline I need placing them side by side on a flat plate.  I will look up how to generate the outline sketch from the body.  In retrospect it might have been easier to extrude the plates using an outline as part of the top sketch and then just offset the starting point of the extrudes - a little more work keeping track of the heights of things but would make later operations easier.  BTW, I don't need linkage back to the original model as I will making any adjustments in the original model.

[etfrench]

I don't think putting them in a different file is the best way to do it.  I would just create a new component, then place copies of each original part in the new component.  Use planar joints or the Arrange function to position them for machining.

[laughingcreek]

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@jhackney1972 wrote:

The OP had this line in his last post " I want to make some adjustments to the outlines - mainly offsets to allow for the kerf of the cut and leave some additional material for finish milling."

...I am wondering how he will be able to edit the sketch, for each component, and have the component update? ...

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missing the point.  the op wants to make changes to the part for purposes manufacture.  this needs to be a one way connection, as opposed to the 2 way connection provided by using a linked component.  he can easily make changes to a derived part that might be needed (offsets, allowances for kerfs, etc) without making changes to the original sketches.   Might need access to the original sketches for some of this as references for anything new to be  performed on the part.  that also can be derived in.  

I have to do this all the time.  I will frequently have an assembly consisting of multiple sub components, and each may have a different workflow for manufacture.  somethings are milled, some are laser cut, some are scaled to be a casting master and sent off to a 3d printer, etc.   Each going to a different supplier with different needs for the file.  along the way prototypes have to be made and iterated.   those aren't always made the same way as the final part, so a different set of files.  I find it's easiest to keep a single file of the model in it's finished form, and derive various bits out for the purposes of preparing for manufacture (splitting into multiple bodies for printing, scaling for casting masters, separating bits that need to be milled or cut, adding extra material for parts that will need to be hand finished, etc.)  if I do all this by pulling out linked components, or if I keep all the operations in a single assembly, it quickly becomes a huge mess.