I have started a new drawing and inserted the front view of the part. The view boundary is nice and tight around the part. I then rotated the view 120° and the view boundaries get much bigger. Now when I insert a section view the A-A cut line extends way too far. It is my understanding there is no way to manually adjust the view boundaries? How do you correct this?
SolidworksDrawings And Detailing
Hover your cursor over the end of the arrow Edit: end corner on your A-A cut line. You'll get a little section line symbol with an end point; slowly click on the end point of the arrow and it will allow you to drag the end point of the line to re-size your section.
As to the view resizing when you rotate it... I shall refrain from addressing that issue after witnessing the unleashing of the Forum Wrath upon another poster who advocated rotating a view on a drawing.
You can also right-click the section line and select "edit sketch" or "edit cutting line" (I've seen both options but I'm not sure what causes one to show up rather than the other). You can then move the line segment as you would any normal sketch line, then rebuild when you're done moving it.
This worked for me, but is there a way to lock in the rotation of the cutline so I am only moving the endpoint of the cutline vertical/horizontal? It seems to move in a freeform mode.
I gave this a try but I couldn't seem to shorten the length of the cutline in this mode?
You can add relations and dimensions like in a normal sketch, but you will have to hide the dimensions to keep them from showing up in the drawing. When I draw a section line at an angle, I often will make it parallel to a line in the drawing view so it doesn't accidentally get moved.
When you click and drag on the A-A section line does it move the whole section line? If so, you have to be very precise about clicking and dragging on just that end point at the corner where the arrow goes 90 degrees to the section line. It's kind of touchy...much like the slow-click technique for grabbing dimension leaders to re-attach dangling dimensions.
Ok thanks that worked. I found it easiest to go to the "Design Tree" on the left, expand section A-A, then right click on "Cutting line A-A" and select "Edit Sketch".
I've seen both too. The ''Edit cutting line'' one has a bug built into it, if you press escape on your keyboard instead of going in the featuremanager to press either the x or the ''Edit sketch'' button, the program crashes. Didn't report it, just like you I couldn't figure out what causes one to show up rather than the other.
Yes I was just moving the endpoint, not the whole line. I found adding a parallel relation worked to keep it vertical as per Austin's suggestion above.
One last thing, to lock rotation using the aforementioned technique you'd need to create your section line by sketching in a line, and constraining that line with relations. Then when you go to re-size it, it will maintain those constraints, and it shouldn't allow rotation of the cut line.
Alex - I also stumbled across the "Auto-crash" feature...
Not sure if I should, but may I ask why it is frowned upon to rotate a drawing view?
here is something you can do
1. sketch a line in your rotated view.
2. make the line "horizontal", and observe the results.
Yes I did this earlier and noticed the line follows the view orientation and NOT the sheet.
This was said somewhat in jest; however, the phrase I remember seeing was: 'There's a special place in hell for drafters who rotate drawing views." That may not be a perfect quote, but it's very close.
A pain, isn't it? It was a lot more present in 2014 then 2016, to the point that I had to adapt my working methodology accordingly to it so I wouldn't crash and lose progress on whatever I was working on.
I can't remember where or why. It might have been in , but I don't have time to look through all 49 pages looking for it. For what it's worth, I do it frequently.
Same, our shop is stuck in old school's line of thought so we end up rotating most of the section views to have them be in the worker's perspective. It makes a ton of sense when you see it but it doesn't follow the ANSI standard as a whole.
This is what I mean, the Coupe E-E and Coupe B-B.
I finally remembered. Someone reported having problems when another user updated the standard views in the model and it ruined the rotated drawing view. That user recommended using Relative Views instead. I'll agree that using Relative View would alleviate that problem, but as I think about it, if someone updates the standard views in the model it would wreak havoc with any existing drawing views except those inserted as Relative Views.
or custom named views
Honestly, why would someone ever update the standard views? That is one of those things that would make my blood boil lol
The only reason I know of is if someone doesn't want to go back and fix the model.