The below pic shows I am trying to do a section view with multiple depth offsets(staircase). The projected section view is larger in length. I assume fusion is adding the vertical staircase cutting lines to the length of the part. I assume this b/c the left part surface and left hole are lined up correctly. Am I doing this wrong or is this something that may need to be looked at?
Drawing section view larger than parent
I reported this a while ago here.. Just testing today and it in my test, if the section line steps are parallel with the section arrows, vertical in your cast the section view should not include the vertical sections. Any chance the vertical lines are not quite vertical?
Here's my test and you can see the sectioned view is 22mm the same as the projected view at the bottom.
Mark
Mark Hughes
Owner, Hughes Tooling
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Just did another test and it seems like the horizontal lines can cause the problem as well. In the image below the line snapped to the midpoint of a line causing the horizontal line to be not quite horizontal and then I get the stretched section view. So while drawing your section line did the snap to the centres of the holes pull any lines out of horizontal\vertical?
Mark
Mark Hughes
Owner, Hughes Tooling
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Hey there. This isn't a vertical issue imho. I think I found the issue and in general it deals with making sure you don't enter and/or exit a part with two co-linear lines(redundant) and making sure you don't cut thru the middle of a hole if not necessary.
This is best described visually. My key takeaways are: Don't enter or exit the section cut lines with two separate co-linear lines and don't end a line inside a hole.
I have no problem creating sections through the centre of holes. What I might not have got across well above is all changes in direction of the section line need to be exactly 90°. If when you snap to the centre you where slightly off the angle is not 90° and the section view will be generated using the total length of the section lines.
Here's my example where I've been very careful to keep all angles at 90°.
Also after the section's generated you can drag the points around and the length of section view remains the same.
Mark
Mark Hughes
Owner, Hughes Tooling
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I see what you mean in the first example with 2 collinear lines and I guess that would fall into the rule where all the lines in the section need to meet at 90° or the section view will be the length of all the lines.
Mark
Mark Hughes
Owner, Hughes Tooling
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@sendithard wrote:
When you slice thru a hole as you did 2 posts above and get the correct length the only issue is your hole representation on the projected section view is half diameter on a vertical cut and a % less as your line, slope changes.
Well that is correct, the section's only through half of the hole. If you turn on hidden detail you can see the hidden part.
When your section view gets incorrectly drawn and becomes larger is falsely appears the hole diam is correct as in your post above this. That was my concern with slicing in the middle of a hole. Look at your post 2 above this each diameter is projecting differently while the part length is accurate. The only diam correct is your rightmost hole.
When the length of the view is increased because all lines are not at 90° the section line is unfolded, so the hole diameter looks correct as you see the section created by both lines passing through the circle. Imagine cutting along the section lines then laying flat.
Mark Hughes
Owner, Hughes Tooling
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