I am trying to model the profile of a rod.
I have two separate sketches as I will be creating a sweep over.
How do I go about aligning the center of the circle to the line on the sketch behind?
Thanks in advance
3d sketches are a bit tricky. If you create a 3d sketch plane you also have to constrain it.
I'll try and illustrate with example
With a normal reference plane this 2d sketch is fully defined
The circle is coincident with the point and the center is horizontal to the point (the equal is to the circle in 3d sketch)
In the 3d sketch these relations are not enough to fully define the sketch
This is because the plane itself is free to revolve as it only has perpendicular and coincident relations..
So an extra relation is required, here an along z on the two points does the job
Hope that helps
If you're using a later version of SolidWorks (not sure when it came in) you can just have the one path sketch & select circular profile & enter a size as below.
Otherwise edit your path sketch & make sure the end point is touching the plane the profile sketch is on, by Ctrl selecting the end point & plane & choosing Coincident. Then just edit your profile sketch, Ctrl select the end point of the path & the center of your profile & select Coincident again or you can select the center of profile & the line itself & choose pierce.
Kevin Pymm wrote: Dom,If you're using a later version of SolidWorks (not sure when it came in) you can just have the one path sketch & select circular profile & enter a size as below.
Kevin Pymm wrote:
Thanks for your reply Kevin.
I haven't explained myself properly; apologies.
I do not want the profile to be aligned with the center of the circle. I want the sweep such that path is on the inside edge of the rod. So the outside edge of the circle would be coincident with the path.
Deepak is correct. I am using 2016.
maybe like this?
Is the suggestion to draw in a construction line and then give it a parallel constraint?
I think I have found my problem,
If I use the 'Insert plane in to 3d sketch' option, (Yellow plane) my sketches do not snap to the lines behind them.
If I insert a plane from the 'reference geometry' (blue plane) the lines do snap.
What is the difference between these two planes?
Thanks for your help Rob!
The principle is the same. Select the edge of your profile & the end point of the line & add a coincident mate. Then you will need to control the size & position of your profile either with dimensions or other sketch geometry as Rob Edwards has shown.
A 3D sketch plane is generally used for controlling geometry within a 3D sketch, although I've not had much use for them myself.
Thanks for the input Kevin!
You can also add pierce relation in centerline endpoint and path. Have a look on the attached jpg
This is also very helpful. Thanks Jitendra!
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