Hello
Have you tried checking or unchecking the options in the section view? I'm thinking of the "Section" option in particular. (see screenshot)
Have a nice day.
vue_en_coupe.jpg
Hello
Have you tried checking or unchecking the options in the section view? I'm thinking of the "Section" option in particular. (see screenshot)
Have a nice day.
Here is an image! I miss something very strong. The "section" option is unchecked!
Do you have any other solution?
Indeed!
When zooming in, these lines don't appear either? It looks like a SolidWorks bug...
This may be because the pieces at that point in the section overlap. Check the assembly with the "Interference Detection" function. If so, you can exclude (not cut) the part from your view in the drawing.
Kind regards
Hello
put the dots and then you can choose the parameters of your line with a right click if you want the line in full.
quite a few good leads have been given to you (note imported parts with errors or interferences) however I am also thinking of another option: in your drawing go to tools, option, document properties, image quality and increase the slider "Wireframe image resolution and high quality LCS/LCA"
Hi everyone! Thank you for all these answers!
I will try to answer in order:
-when zooming in the very don't appear either
-some pieces overlap but not in the place where I am missing features
- no imported geometry
-I tried to move the cut marks
-I have interference but I have to, I laminate the material in places
- the image quality is already at maximum
So I still have the problem, do you have any other leads?
If you switch your drawing view to shaded mode, the lines appear?
I just saw that if I click on "show/hide" the invisible lines appear in orange, but I validate nothing happens
in shaded image the lines are visible, but I can't print in shaded image
When you do a Show Hide, you have to click on the stop to show and validate so that it reappears when you leave the Show Hide
Mickael
If you click on the orange edges in "show/hide" mode, it should make them reappear or otherwise you right-click in the "Property" view and then on the "show hidden edges" tab, you delete all the edges present in the insert
Your last two proposals don't work! on the other hand I found a backup solution, by unchecking the case "Hide the ... "
Here's where to find the box. On the other hand, if you ever think of another solution, I'll take it
But in fact, this is a flattened cross-sectional view?
it is an ordinary cross-sectional view
Hello
That's why I asked you this:
When you create a cross-section by multiple strokes in SolidWorks 2013, normally a menu asks you if you want to create a flattened section or a "normal" section.
In the properties of a normal cut, you will not have the option to hide or not the cut line breaks.
If by mistake, you checked: Don't show anymore when you got the message asking you what type of cut to make, you could have created a flattened cut without wanting to.
In the SolidWorks options, Messages\Error... The option for flattened cuts to be ticked is:
Alert New feature for cross-sectional view...
If you then make a cut again in several strokes, the choice of cut will be requested again.
I am attaching a video, but it may not be your problem.
Mickael