Fusion
One of your edges is an arc, is it supposed to be? None of your sketches are fully constrained, if you'd made this sketch fully constrained you would have spotted the error.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Just a heads up on a few things after looking at the design a bit more.
There's no need to use offset face to change the length of the flanges from each end. You can set offsets for the edge in the flange feature. Also you can do both sides in one flange feature.
Only 7 features to create the part, see attached file. I guess you exported this from another assembly looking at the sketches?
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
@andrei8XEXS wrote:
Hi
Thanks a lot for help!
My intention is to create the lateral shape of the competent with 2 lines and an arch (the upper part of the laterals).
I'm not very experience user so if you can detail a little bit what can I do in order not to start all over again, I will be grateful!
Andrei
My guess is when you created the arc you did a click and drag movement rather than clicking one point then the next. With the line tool active if you click and drag from and existing curve Fusion will add an arc. All you need to do is delete the arc then recreate using a line.
To fix, edit the sketch and delete the arc and replace with a line and add a tangent constraint between the line and arc.
The sketch is still not showing as fully constrained because you have a construction line created when the drew the 45° line. One easy fix is just drag the point on the bottom line to the centre line.
Now you should have a padlock on the sketch showing it's fully constrained.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
@andrei8XEXS wrote:
Great suggestion!
Edit, just testing and this doesn't seem to work if I change the parameter. I'll report this as a bug in another thread.
Edit, not a bug, I forgot to update both edges. See new updated design attached.
One more suggesting. To make the part easier to edit, create a parameter for the offset ends of the flange. Then use the parameter in the flange feature so just editing the one parameter updates the offset on both flanges. See updated file.
Mark Hughes
Owner, Hughes Tooling
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
