How to have multiple instances of a feature (besides patterns)?

[luca.giorcelli]

Ref. this design: http://a360.co/2cIQIsv

I have the following "cut" feature repeated many times on different bodies all around my design.

MY CURRENT WORKFLOW (SUB-OPTIMAL?)
As you can see, my geometry (many bodies with different patterns on each one) does not allow me to replicate a "unique master feature" relying on patterns only. So, at the moment, in my workflow I have to manually duplicate the original feature, as follows:

1. For any target body I create a new sketch and I manually re-draw the same cutting geometry

2. I cut the target body and I apply some fillet

3. I multiply the cut on the target body using patterns

MY QUESTION
I guess taht this workflow is not optimal because it relies upon duplicated sketches/features instead of referencing a unique master. Can you suggest me a better workflow avoiding sketch/feature duplication?

[TrippyLighting · Accepted solution]

Create this feature as a solid body within a component.

1. Copy/paste that component as often as needed and assemble these copies to the the desired location(s).
2. Use the "Modify->Combine (cut)" tool to cut all instances of that copied component out of your main body.
   This absorbs all the bodies in the previously copied feature component,
3. You an use "Remove" to eliminate these unwanted components from the browser.

If you want to modify the cut-away component, you need to locate and edit the sketch for it in the browser.

You can also move the timeline marker back to right after the point of creation of that component and add more geometry to it, if editing the sketch is not enough.

This will modify all the copied components as well.

This method would also allow to create a number of re-usable library features.

[JYZMT]

Hello, I have a question on a very similar workflow. I understand the previous answer, and will use it unless there is a cleaner answer to this question....  I need holes at the top of all these bodies. 

 

I was trying to use the pattern feature along a path, with a hole feature. Using some quite painful maths, I have an equation which works out the spacing, and I have a vector for the direction. I created the holes, using the hole feature, and tried to use pattern along a path to apply to multiple bodies 

BUT, because now the hole function has the 'objects to cut' dialogue, and I can't add bodies to it that it does not effect at that time, using the pattern hole along path does not work, because it ignores the other bodies.

Neither does making the the circles in the sketch, then using the extrude feature to make the recessess and holes , then also trying the pattern feature along path. Again this has a "apply to objects", which stops the extrude applying to subsequent bodies.

Is my only option, as per the previous answer, to make a subtraction component, copy and paste to multiple locations, and then subtract using the combine? 

Thanks

[davebYYPCU]

We can make best guesses without your data,  

looks like each board is getting longer along the path, could be wrong, 

Are you putting the holes in the first body, before the duplication in your timeline?

Or trying to place them into each board after the duplication?

[JYZMT]

Hello, Thanks for your time. Yes each fin gets longer. Each fin is made from two boards. 

I made all the boards from a couple of extrusions of a sketch. So they are individual bodies. Then I made another sketch to set out the holes. Then I tried to pattern the holes up with the diagonal vector. But this did not work. 

These fit underneath a stairs. And so the pattern along a path has been very useful before on this model. For example, I made a single tooth of a cut stringer, combined these to a body, then patterned the combine feature up the stringer. This means I can change the number of risers in the stair and everything adapts. Its working really well. BUT, in the stair stringer, the combine feature is applying to a single body, not multiple unrelated bodies. 

This pattern along a part work flow works well for the stairs, but I'm not convinced  I'm working in the best way for the parts underneath, because although they have the same operations made to them, each one is different, and its taken a boring evening to re apply the same operations to every Fin. 

I ended up making a new component that contained only a sketch. Then using move/copy (point to point) to duplicate it to the end of each fin, and then apply the holes to every sketch. I did the the same for the rebates that take the shelves. It all works, but, it will fall over if I add or remove steps (where as the main body of the stair copes with this fine.)

It feels like there should be a way to select all the bodies, and say "do this to operation all the ends" or something like that?

Also I should note that this modeling has crashed fusion out a good few times today. I ended up making a new file, and linking in the main stair body, then building the shelving below in the new model - this proved much more stable. Of course, it could be the way I built it. 

[TrippyLighting]

And the design is still not linked or attached beasue ?

[JYZMT]

Firstly because I could not work out how to do that. Can I link direct from the cloud drive, or do I need to export and then upload?

And secondly because in the time it took to write the last reply, When I went back to fusion its has hung. Again.

I know. I should have saved it before. Its midnight here. I'll have to sort it in the morning now. Thanks anyway 

[davebYYPCU]

If you have linked components, you share a link from the cloud, (xxx.f3z) paste the link here

if the file is stand alone, (xxx.f3d)

File > Export to the hard drive and select it in the attachment box of this system, 

Something to sleep on, do all the operations you need before the pattern that works.

Changing the workflow order will be all it takes.

Might help....