Problems getting multiple bodies to combine together

[Anonymous]

Hi All,

I am pretty new to Fusion, and have been having a hard time with what seems like a simple operation. I had a part that was slightly too big for my needs. I broke it down to a single body, fixed the sizing issues, then re-patterned it. I thought the combine function would then join the bodies together, but this did not work. Please see the screencast for an example of what I tried.

Thank You,

Tony

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[davebYYPCU]

Imported / non Fusion Geometry?

Edit to a Base Feature?

Or Sketch a Rectangle and Extrude it.

Might help....

[laughingcreek]

A number of possibilities, but just a guessing game without the model.  probably something to do with the pacing on your pattern.  certainly achieving what you want to do will be easy enough, even if by some other process.

file-export your .f3d file and attach for specific help.

[Anonymous]

Hi,

Here is the file shown above. I did try to investigate the spacing after the patterning. When I measure between the bodies, the distance lists as 0.0.

Thank You,

Tony

[Anonymous]

Hi,

You are correct that the original model was just imported into Fusion. I tried to edit the base model, but I dont see how that would effect the downstream steps I took in this case. I am pretty new to fusion, so maybe im missing something?

Im also not sure how extruding a rectangle would help. For clarity, there are internal structures in each box. I attached the .F3d file to another reply.Any further thoughts would be appreciated.

Thank You,

Tony

[laughingcreek]

You didn't go out enough decimal places.  I get .012 mm between, which makes sense because the edge length is 31.988, but you patterned at 32.

attached is a hacky fix that may be good enough.  add a little bit to one side with push pull, pattern, then take that little bit back off after the combine.

[TheCADWhisperer]

I would have done this entirely differently, but for your immediate issue - if you zoom wayyy in, you will see gap between the bodies.

Frankly, I recommend that you start over - starting with a fully defined sketch at the Origin.

I recommend that you never ever use Fix constraint (at least not for the next 6-18 mths).

There is almost always a better technique.

[laughingcreek · Accepted solution]

you can also turn the general precision up all the way in preferences.  then use the measure function in the dialog to measure the edge for spacing.

see attached.

or even better to turn up precision and then actually fix the original body to be actually 32 mm.

[Anonymous]

Thank you, I combined a couple of these responses to fix the issue. I will definitely be more aware of the extra precision needed in the future. I ended up going back to the beginning, re-sketching the cuts i needed, and then repeating the patterning and joining, which worked correctly this time.

[Anonymous]

Out of curiosity, why would you avoid using the Fix constraint option?

[TheCADWhisperer]

Not needed.

I tie my geometry to the Origin (or to another part tied to the origin).

The only fixed, absolute position is the Origin.

I use the BORN Technique in modeling.