I am currently making several technical drawings with the " Drawing " function of SolidWorks 2012. On the main view (front view) of a part in revolution, there is a hole with a bore and a chamfer, right in the middle of my part. I would like to make cross-sectional views of all degrees around the central point of my hole. When I draw the line of the cross-sectional view, I have to manually move it to get the passage positioning in the center of my hole. But when I zoom in, I notice that several cross-sectional lines of sight are not positioned precisely in the center of the hole. (see attachment)
Can you tell me the method of positioning all my lines of sight in section at the same point (center of the hole) even when zooming in ?
This will avoid manually positioning them with the associated uncertainties.
You have to right-click on the cut line => edit the sketch. Then in your sketch you have to place a point in the center of your hole (it will unfortunately be visible later. I haven't been able to hide that yet) and then make a coincidence between your dot and the line. You validate your sketch and TADA!
First of all, the view you show in 200x zoom does not necessarily mean that your lines do not pass through the center. It may simply be an inaccuracy due to the graphic quality you have set for your document.
To know if your line goes through the center, you need to edit the sketch of your section and make sure that it is constrained (black line and not blue). To constrain it easily and in your specific case (centered and symmetrical part) I will select the midpoint of your cut line (right click on the line, Midpoint) and make it coaxial to the drilling. All you have to do is give the orientation of this line with a corner dimension.
In the case of a non-symmetrical part, I will place a coaxial point at the hole and make the line coincident with this point. All that remains is to constrain the orientation as for the other method.
Edit: too long to write, answer from @coin37coin in the meantime!
To complete what coin37coin says, instead of creating a point that will stay on the plane, you just have to make the temporary axes of the part appear and constrain the cut line on them (see attached image).
@Rim-b the problem of temporary axes... it's because they're temporary!
What I mean by that is that if you change your hole in place, the axis doesn't necessarily follow. I'm fooled in 3D by doing placement in relation to its axes. As soon as I modified a little, my constraints were broken and no longer followed.
After that, Solidworks may have made an evolution since 2011 and solved this problem?
I'm in the 2012 version and I just did the test on a piercing. I constrained a cutting line on the temporary axis and I varied the size and position of this hole. I haven't lost my constraint on the drawing. Apparently this problem has been corrected since the 2011 version.