Hi, I am new to Solidworks 2017 and am currently geared towards Creo. I would like to simply select sketch references on the face of a part (edges, plane intersections, circles, etc) so that my sketch geometry will snap properly in place. Thanks.
Corey - you can click a blue vertex and drag it over the edge and it should snap to an alignment.
As for symmetry, you need to select two vertices and the centerline (in any order) and the symmetry relation will pop-up.
I would start here:
Can you describe a specific problem? Perhaps with a screenshot to explain what it is you're trying to achieve?
when you have a sketch tool active (like line tool) when your sketching on a face, hover over any edge, vertex to snap to it. keep any eye on what the feedback is telling you next to the cursor. there is a symbol that shows up for edge, vertex and face.
So I am trying to sketch a rectangle on the surface of a bushing (see below). The rectangle needs to be symmetric about the centerline and have all 4 corners coincident to the circle. I need to also draw the arc section between the vertical entities of the rectangle. (In other words, this rectangle represents a saw blade cut to halve the bushing. In creo, if you created a centerline and established the first corner of the rectangle, the second corner would snap to the other side of the circle and recognize the symmetry about the centerline. Then I could just trim the outer circle in order to keep the arc length between the cut sketch. Thanks in advance.
Thanks Nate, this seems like a good way to do it. I also just found that the "center rectangle" command works well to. I think the main issue for me is the learning curve and trying to detour from my usual processes in Creo. Thanks again!
no problem - I feel your pain. I was a Pro/E rat for 18 years before I touched SWX - I still use Creo for one client, but I actually have fully transitioned to loving Solidworks and (almost) hating PTC. Well, they both infuriate me at times. I guess we'll never be rid of that.
Corey.. click on the line and RMB,.. a pop up menu will provide a "midpoint" option.. select.. then a orange mid dot will appear.. then ctrl/select your centerline.. and apply your coincident contraint. (mp4 attached)
Sketch geometry will snap into place if these options are enabled at Tools > Options > Sketch > Relations/Snaps.
Hi Corey - welcome to SolidWorks! SWX sketcher constraints work sort of backwards from ProE. As you're sketching, the cursor shows you inferences that the sketcher will make for you . Yellow icons will stick and be applied to the sketch, but white icons will put the geometry as is implied, but the constraint will not stick.
Then, as you select entities, the instant pop-up dialog that shows when you let go of the click will present to you the various constraints available for what is selected (e.g. an arc selected will not show a vertical constraint...etc)
OK - I am not going to baby you anymore with the Creo terminology. These are called "Relations" now. What you used to know as "relations" are now called "equations" (You will find that similar learnings will be needed for family tables, parameters, etc...)
The beauty that you need to force yourself to appreciate is that you don't need to pre-select your sketching "references" - SolidWorks treats ALL existing geometry as a potential for a relation reference. However, the automatic inferring of a relation sometimes needs to be coerced - or taught. For example - if you want to relate an end point of a line to the center of an existing round hole, you may need to hover your cursor over the edge of the hole until you're shown some dashed geometry highlighting the holes center and edges. Once you see this highlight, you can confidently move your cursor to the center and the endpoint you're dragging will get snapped to the center.
Also - you will find frustrating (even after 5 years of heavy SWX use, I still do...) SWX will not use a planar face for relation reference geometry. You will be FORCED to use edges for reference geometry in a sketch. Yes, even the tangent edges of fillets.
Hope this helps some...
As Dan Pihlaja suggested, you'd better go thru the tutorial from your SW software
in the mean time, you can drag any entity such as line, point and they will be snapped to the other existing entities (with the snap option on)
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