unable to break line on one face but when i draw the same thing on another face it does it automatically

[fushikoshi]

I am unable to break a line on one face of the design but it seems to automaticly break or merge sketches on another face of the drawing. This prevents me from filleting on one side of the drawing

[jhackney1972]

Please attach your model so the Forum users can take a look and advise.  If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section, of a forum post, to attach it.

[hamid.sh.]

Please share your file (export to *.f3d). Also instead of attaching pictures (which is hard to view) please use Insert Photos button, or simply paste it:

[davebYYPCU]

Both sides of the model are not the same, you can fillet left edge, but right edge is not there.

Might help.....

[fushikoshi]

Please see attached 

[fushikoshi]

Thank you, I have posted the file.

[fushikoshi]

Yes, the problem is I drew each side exactly the same way, I even deleted everything and redrew it to be sure. For some reason I can't figure out why the rightside automaticly makes a seamless face and the left side does not.

[TheCADWhisperer · Accepted solution]

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@fushikoshi wrote:

Yes, the problem is I drew each side exactly the same way...

Sketch1 is not fully defined?

Use equal (=) constraints rather than duplicate dimensions.

Blue geometry (under defined) should keep you awake at night.

Sketch3 is not fully defined?

Use sketch Slot for slot shaped geometry.

Sketch4 is not fully defined.

Do not repeat sketches - duplication not needed.

Zoom in on Sketch3.

They are not exactly the same.

Circle is not tangent to edge.

Sketch1 should (almost) always be at the Origin.

Corrected file to follow in a few minutes... ...check back.

Two circles at the Origin.

One line Midpoint to the Origin and one dimension (any time you are duplicating dimensions you are probably doing too much work - get lazy - don't do extra work.

Tangent angled lines do not need dimensions - get lazy.

Use Construction lines (not technically needed but provide visual indication of true Design Intent).

One dimension.

Project construction line (or one of the two horizontal lines if the construction line not used).

Search Google on BORN Technique and then use as much as possible and practical.

BORN Technique.

Use Slot sketch and do not repeat sketches - get lazy!

Extrude and Extrude Cut or Extrude and Mirror.  Did I mention, get lazy?  Do not repeat work.

Do it once.  Do it right. Robust and predictable behavior on edit.

See Attached file...

[fushikoshi]

Thanks for a quick reply, I got a little stuck getting the vertical/horizontal constraints to work. The only way I could complete the sketch was by using dimensions.

I also couldnt figure out how you acomplished the extrusion.

 

 

 

[TheCADWhisperer]

Remember I said to Get Lazy and NOT use duplicate dimensions?

What happens if you delete the duplicate dimensions and then drag the unconstrained endpoints?

Do you observe that the construction line is missing a Horizontal Constraint?

Do you observe that the "vertical" line on the left side of this image is missing a Vertical Constraint?

[TheCADWhisperer]

Is your Sketch2 fully defined?

Remember how I said that blue geometry should keep you awake at night?

You should have stopped at each issue and asked questions as they occurred.

Not only should blue sketch geometry keep you awake at night - you should also not be able to eat or play (however  you want to define "play").  You should just be focused on determining what is needed to constrain your geometry.

[TheCADWhisperer]

Speaking of the power of observation -

do you observe anything different in the dialog box for my Extrusion vs the image you posted for your Extrusion?

Tip:  See Green box vs red box in image above.

If you click on the image it should get larger so that you can more clearly see.

Are you starting to see how this is all based on logic.

BTW - for future reference  you should be posting your questions over here >>https://forums.autodesk.com/t5/fusion-360-design-validate/bd-p/124<<

This "Support" area of the forum is more for reporting bugs in the software.  (I know - it is confusing the way they have set this up.)

[fushikoshi]

Sorry I missed the join step before the cut step.

I am getting a feel for the process but seem to be having a difficult time with anything to do with constraints.

For sketch 2 I have no idea what else I could define to complete the sketch. I have all the nessissary dimensions I can see and the left side coincident to the construction plane.

As for sketch 1 constraints I can't figure out how to get the same constraints as you did. I have spent a while trying deifferent combinations and deleting different things with no luck.

Yours

Mine (just one outcome, I tried many different things but noting looks like yours)

I just did a quick screencast but kept getting an error when I inserted it into this message so hopefully I explaind my issue enough.

[davebYYPCU]

For sketch 2 I have no idea what else I could define to complete the sketch. I have all the necessary dimensions I can see and the left side coincident to the construction plane.

I don't think so, if it's blue, click and drag it.

One more constraint to go.....

and for fully defined, delete the 90 degrees dimension, and make any vertical line vertical.

Might help.....

[fushikoshi]

Thank you it seems like its the order constraints and dimentions are added is key.

After redrawing it this morning I figured out that if I add the conicident before I add the 16mm on sketch 2 it works.

Thank everyone for all the help, I truely appriciate it.

[davebYYPCU]

Gotta ask why did you redraw it?

We recommend - constrain everything you can, then dimension what’s left, per sketch article.

You should never Finish sketch before the icon gets the red tick.  

might help....