When I tried to connect these two points by a line following result is coming. What is the reason? How to fix it?
3d sketches have tons of possible relations to show up during the sketch process.
I would recommend under system options turning off automatic relations in your sketches.This is easy enough to toggle on/off when switching back to 2d sketches.
I used to use the control method that Glenn Schroeder mentioned above, but for some reason now it doesn't work for me either. I do know turning off the automatic relations allows you to assign as you need to in a 3d sketch pretty easily.
Delete the relation shown in the screenshot below. You can find this error solution the same way that was explained in your previous post by using Sketch Xpert
It worked okay for me. You might try again, but this time hold down Ctrl while placing the sketch. That will disable automatic relations, which can be helpful sometimes, especially when working with 3d sketches.
Can you elaborate on how to do this? It sounds so simple yet when I hold ctrl it won't let me sketch anything.
Same as for me. when I hold ctrl it won't snap to the point.
Yeah maybe it's a setting. On a different note you can also choose the coordinate system setting your line follows by pressing tab before you connect your line. This will work too although I would much rather have the ctrl solution work. Hopefully we can clear this up
Maha Nadarasa wrote: Same as for me. when I hold ctrl it won't snap to the point.
Maha Nadarasa wrote:
That's the whole point. If you place sketch entities while holding down Ctrl then no relations are set. Not coincident, parallel, along X, nothing. Sketch your line first with Ctrl held down, then release Ctrl, click on the ends of the lines, and drag them where you want. They should snap to coincident with the other line ends.
I suggested this for 3d sketches since it's so easy to get unintended relations when working with them.
And Derek, I don't know why it's not working for you. It should be just as simple as it sounds. Hold down Ctrl, then place the sketch entities with your cursor just like always.
Maybe I didn't explain myself clear enough. When I am holding down ctrl I can't sketch anything. Maybe its my workflow so let me run that down and see what you think. I am in his 3D sketch > press s key > select line tool > hold ctrl and can't draw a line at all anywhere. It's like it completely disables the tool. On the other hand I can draw a line as I normally would and then drag to the points like you recommended and it still doesn't add relations and gives me a fully defined sketch.
Same as for me.
try the shift key, not the control key
OK, I tried that and it doesn't work and still adds relations when drawing a line from point to point. When I do this and draw a line in space and then connect the points it doesn't add relations, but it also doesn't add relations when I do this without the extra of holding down shift or ctrl. IMO he has plenty of solutions to get him a defined sketch. In a perfect world it would be nice to be able to draw a line holding ctrl or shift while snapping to points but not adding relations such as parallel, perpendicular etc. If the solution is to hold ctrl or shift while drawing a line in space and then connecting points but it also works without either of these extra keys being pressed I am not seeing a point.
So solutions I see suggested here are.
1) draw a line in space and then connect points to avoid the addition of relations
2) draw a line and use tab before connecting the last point so you can choose the correct plane the line follows thus avoiding over defining relations
3) delete the over defining relations causing errors after sketch is complete
Is the only way to toggle this off and on when switching from 2D to 3D changing this system option every time or is there a shortcut? Would be nice if they could be set independently for 2D and 3D sketches.
This is the only way I have used it. I did this alot when I started in structural weldments years ago. I don't use it anymore because I typically just draw my lines and drag them where they need to be or I keep an eye on my relationship buildups so I don't see the overdefining as much as when I started out.
This process for developing 3d sketches and weldments is one that takes time and practice, you are going about it the right way from the standpoint of asking questions when the issues arise. Patience is a virtue in these models as they will get cumbersome and bigger as you develop more complex structures.
I found another way of doing. Sketch the line from 1st point only and choose other point (we say point3) randomly then apply coincident relation between point3 and point2. It worked but I couldn’t explain it how.
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