Convert Entities Workaround?

[CruftMeister]

Howdy Fusion360 Community - 

While I laud the Fusion360 team for knocking off a lot of issues thereby making the package much more functional and easy to use - this topic pertains to a Solidworks function that I really miss and don't expect to see in Fusion any time soon (if ever) so I'm looking for a Fusion360 workaround.

What I'd like to do is be able to capture the profile of some geometry in the sketching plane, and then be able to modify that profile. I routinely did this in Solidworks with the "Convert Entities" (essentially a zero value offset) command and while I know the Fusion mantra is "You shouldn't need to trim geometry in Fusion." I'm struggling to find a good clean (easy) way to replicate the utility of Convert Entities.

To give a very simple example of where this approach would be handy, I've inlined a screenshot of a simple F360 model, were I want to filet the corners of a rectangular extrusion, but only partway along the lengths of the corner - it was a simple CAM demo file.

As you can see, I was able to accomplish what I wanted, but the way I did it was not very clean - I offset the geometry in the sketcher, then added filets, which broke the constraint to the model geometry, and I then used the co-linear tool on the sketch palette to constrain the line segments to the edges of the geometry.  While this method can be made to work - albeit with a lot more steps -  on simple geometry, if you try this on more complex geometry, with arcs and splines, especially if it is say a STEP import, it really won't work well.

I'm sure there are a number of better ways to do this in Fusion - any thoughts would be appreciated.

Thanks!

[davebYYPCU]

As a Fusion self taught user, never used Solidworks,

you have only slightly confused me, but there are a nmber of ways to make that block in Fusion, as stated, without Convert Entities,

which I presume is our Project command/s.

The easiest way with one sketch, filleted corners with the square sides extended, extrude the filleted section up, and the square section down, with second extrude as Join.

If the sketch is on either top or bottom of the block, extrude half way, then new extrude new body, them Model fillet the top block, and combine Join for a single result.

I didn't see a need for the Project Command in this example, hence my little bit of confusion.

I have also taken a Zero Offset surface body from the side of the block, shows the text above in one pic.

Might help....

[CruftMeister]

Hi Dave,

Thanks, those are certainly viable workarounds to build the same end result, but, the methodology sort of misses my goal of modifying existing geometry, vs making the desired shape from a starting point.  The reasoning is subtle, and not well evidenced by the simple example sketch I used, but imagine trying to do this with more complex geometry, especially if it is imported say from a STEP file. In that case, you would really like the ability to modify the existing geometry because you can't go back and start midway through.

Regarding the need for Project, I started with a square block of geometry and wanted to add the filets, not build the geometry from scratch, hence Project.  As I said the geometry I used was simple to illustrate the question, but try to imagine something more complex, say with splines. 

I am intrigued by the zero offset surface body you show, it looks a bit more involved than Convert Entities, but it might work for the complex and/or imported geometry I mentioned, I will give that a shot.  If it works, that is exactly the sort of thing I am looking for.

Thanks -

[davebYYPCU · Accepted solution]

I still haven't identified what your trouble is, fillet part of an edge? 

you can split the body at the end of proposed fillet, add the fillet and then combine back to single body, no sketches.

Project then Break Link?  Line or curve will take modification but not move unless you move it.

as for - I am intrigued by the zero offset surface body you show, it looks a bit more involved than Convert Entities, 

Can't be more simple than starting the commnad then clicking on the side of the block, set size - defaults to zero, and then OK.  Hide the solid block to see it.

[CruftMeister]

Thanks for your response. I had tried splitting but didn't get the results I wanted.  I tried it again and now realize I must have split the faces not the body - splitting the body does indeed work.

On the zero offset surface body, I can see how it would easily replicate the original geometry (in this case a rectangle), but not sure how to modify the resulting surface (e.g. add the radiuses) so that the result could be projected into a sketch so as to accomplish the desired geometry modifications.

In the actual cases where I needed to modify an existing profile of complex imported surfaces, I ended up spending hours manually breaking links and replacing multiple segments of projected geometry because otherwise you can't touch them in Fusion.  I don't like doing this as it is a huge time suck and results in a brittle model downstream - but yes it can be done.

To me the question is, given that both Pro-E/Creo and Solidworks offer this functionality, what is it that makes the Fusion team so reluctant to add the ability to project geometry that can then be edited. . .

[jeff_strater · Accepted solution]

@CruftMeister,

Here is yet another way to do this:

As to whether we will ever implement editable projected geometry, I can't say.  It's possible.  It's not particularly high priority right now, because we are focusing on things for which there is no other way to achieve the result.  Because fusion is very flexible about how profiles are picked for sketch-based features, there are often a lot of ways to draw your sketch so that trimming in general is not needed.

Jeff

[CruftMeister]

Hi Jeff,

Understood that it is not a priority, though nice to hear it could be implemented at some point down the road.

Your technique is clever, I'm assuming that you just change the offset in the method you show to change the filet size.

Thanks -

[Anonymous]

Have you tried starting sketch on the body, then click sketch/ "project/ include" / project?   it works great for me.  my goal was to export a body to DXF.  But I think fusion limits you to only be able to export a sketch to dxf.  I'm drawing parts to be cut from sheets of carbon fiber. 

Here is where i learned about this function - https://forums.autodesk.com/t5/fusion-360-design-validate/quot-convert-entities-quot-in-fusion-360/t...

Hope this helps you as much as it did me!

[Anonymous]

I am new to Fusion, after a 2 year break from 2-1/2 years of intensive use of SW, and I miss Convert Entities already.