fusion changed a dimension after extrusion

[mi.silva]

Hi all

I have a sketch 1 on Internal Slots component with a function value of 267.00 mm after extrusion this length is changed on the body to 267.004 mm.

Can anybody knows why, project is bellow.

Thanks all

[HughesTooling · Accepted solution]

Your sketch is not fully constrained and is at an angle! The horizontal length is 267mm but because the line is at an angle, its length is 267.004. You need to fully constrain the sketch making sure lines are horizontal and vertical.

[HughesTooling]

How did you end up with no constraints in this sketch? Is it imported or did you delete them?

You'll need to pretty much start again with this sketch because you end up with conflicts when trying to add constraint now because some lines are being held parallel by dimensions and although they are within tolerance they don't end up vertical.

Like here the white vertical line is being made vertical by the 95mm dimension from the end line of the main rectangle but you can see some small error in the jagged 10mm dimension and this causes a small error in the 10mm length. This is all within tolerance for the sketch solver but caused by adding dimensions to lines without horizontal\vertical constraints (your original sketch was skewed and adding constraints after dimensions will not work for small errors). If you'd added all the constraints first then the dimensions it might have worked. 

Something else to avoid is lines on top of lines, for the cutouts use 3 lines not a rectangle.

Mark

[mi.silva]

Yes it was imported from a student to try to save time and not redraw everything but sometimes shortcuts take us the long way. Thank you so much for your replies. 

[HughesTooling]

After a bit more playing around I found the problem with your cutouts is the line that's on top of the line of the main rectangle is not constrained at both ends.

After adding coincident constraints I can now get the sketch fully constrained.