Is there a way to align and lock a circle (drawn with symbolic lines) to a reference plane?
See attached image.
I am building a 2-D Furniture Family, and need the circle (opening in table) to move when the length of the table growa.
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Is there a way to align and lock a circle (drawn with symbolic lines) to a reference plane?
See attached image.
I am building a 2-D Furniture Family, and need the circle (opening in table) to move when the length of the table growa.
If you go to the element properties of the circle you can turn on the center mark and constrain to that.
Steve
Did this end up working? I am having the same issue but dont seem to be able to solve it. I am sure it is a simple thing that I am not doing but could I get some advice?
I am drawing the circular extrusion, making the center mark visible and adding a dimension within the extrusion editor between the reference plane and the center mark. When i go to change the associated parameter i get an error.
I usually do 2 semi-circles. for some reason this works better for me.
Turning ON the visibility of circle's center in its properties and than aligning it and locking to TWO ref planes (vertical and horizontal) always works for me. You can even turn off the centre later if you want too - it's still locked.
I use it quite a lot for doors families and their plan swing lines - all my doors are fully parametric (of course) including the angle of swing. It never fails...
I often wander why these centres are turned off by default anyway? Much more often than not I end up initially turning them on for this purpose then turning them off at the end. One unnecessary step every time I use circles...
I agree and I agree. The main issues I have run into with curves is keeping other lines tangential to curves.
1. Draw reference planes for center.
2. Add dimensions to reference planes.
3. Flex model to make sure the dimensions work.
4. Make extrusion with lines.
5. Draw curve by center, from intersection of reference planes.
6. in 'instance properties' of the curve turn on 'center mark visible'.
7. Use the 'Align' tool to align the center to the reference planes, and lock (both hori and vert)
8. Finish extrusion, and voila...
If you need to make the radius of the circle parametric, use a radial dimension, select and choose a parameter as usual (do this in 'edit' mode)
Peace.
I have drawn a circlular extrusion and aligned it to both the vertical and horizontal planes (locking it each time). When i adjust the dimension the circle moves which is great. However when i add a radial dimension to the circular extrusion so that i can adjust the height of the center of the circle and the radius i get errors. If i remove the the radial dimension the height works again and vice versa if i remove the height dimension the radial dimension works.
Is there a problem with this scenario? Surly you can control both the radius and height of the center of circle with parameters?
The reference plane to which the extrusion is locked is not pinned. The default front/back and left/right planes are pinned. Still got the same issue, extrusion will move providing radial dimension does not exist and vice versa.
Test file attached in which the height and radius parameters are set, if either is changed an error occurs, if the problem constraint is removed the remaining parameter works.
Stumped!
Now it works. What I did was I simply deleted your original ref. plane and created new. I also created another ref. plane - this one inside your extrusion, so you must enter the EDIT MODE to see it. I also aligned and locked the centre of the circle to this second ref. plane. I don't know if this has done the trick, but now it works...