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# Thread: Can circular geometry be controlled with a reference line?

1. ## Can circular geometry be controlled with a reference line?

I want to control a hole's position in an extrusion used for a gusset plate by means of distance and angle from the origin reference planes.
I have made a reference line from the origin and assigned angle and distance parameters which function ok. However the hole in the extrusion will not attach to the end of the reference line and move with it. Neither a circular void will do it. Any solution?

2. Have you tried turning on the center mark of the circle and constraining it? Just glancing at it I would lean towards using formulas to control the location. Since you know the Angle and length of a side you can use some basic trig to solve for the other values. http://www.revitforum.org/tutorials-...day-usage.html

3. Just add the parameter dimensions in sketch mode (for the void). When you start a dimension and hover over the circle, you'll see the center marks appear. It will have to be ortho though (I believe), so some trig will be needed as Chad suggested.

Just remember that you have those parameters in sketch mode, because they won't show up otherwise.

4. You don't need the reference line or any dimensions in sketch mode (unless you want a radius / diameter). To turn on the center mark select your circle, then look in the properties palette - there is a checkbox to turn the center mark on.

5. Originally Posted by dzatto
Just add the parameter dimensions in sketch mode (for the void). ...
Ouch, no, no reference lines, reference planes, dimensions, or parameters in sketch mode, please...

6. ## The key is hosting the circle on the reference line.

If I understood the question correctly, I would use a reference line and here is how. The key is to host the circle on the line. Here are the steps:
(1) Make the reference line.
(2) Give a dimension to the line by selecting its end points and assign the parameter length. (flex)
(3) Give an angle and make it parametric (flex)
(4) Set the horizontal plane of the line as current.
(5) Make a circle with its center as the end point of the line. (Now the circle is hosted on the horizontal plane of the line. If you want, you can highlight the circle and from its properties, turn on the center mark)
(6) If you want, you can make the circle radius also parametric.
(7) Change the parameters and it should work. (See the attached file rvt 2013)
This can then be extruded to make a void.

Hope this helps.

7. Originally Posted by Alfredo Medina
Ouch, no, no reference lines, reference planes, dimensions, or parameters in sketch mode, please...
I totally agree Alf. I just knew you could get to the center of a circle in sketch mode. Chad had the right solution. I totally forgot you could turn on the center mark in properties.

8. Originally Posted by viratmanchanda
... I would use a reference line and here is how. The key is to host the circle on the line. Here are the steps:
(1) Make the reference line.
Here you forgot a step. Before your Step # 2, the start point of the reference line needs to be aligned and locked to the horizontal and vertical reference planes, to prevent the reference line from moving when the value of the Angle parameter changes. (The line is not staying at the pivot point in your sample file. Try changing the angle to 90, then 45).

9. You are right. I missed that one.

10. Thank you everyone.

If I have understood it correctly, there are different approach to control circular holes in extrusions whether you use reference lines or reference planes. I have not found this in the Autodesk Help. A circular hole in an extrusion controlled by a reference line can only be made from a model line circle that act as a reference. Right?

I chose the recipe by viratmanchanda and Alfredo.
I found it a bit more complicated than expected though, especially when handled by a novice like me. So therefore I will rewrite the steps from what I have learned in my tests (RVT 2014):

1. Make the reference line.
2. Lock the one end of the reference line to the vertical and horizontal reference planes (that define origin). It can be difficult to hit the right point while dragging the endpoint. It might be easier if you hide all but the ref. planes and ref. line.
3. Give a dimension to the line by selecting its end points and assign the parameter length. (flex)
4. Give an angle and make it parametric (flex)
5. Set the horizontal plane of the line as current. (or vertical depending on the orientation of the plate on the hosting face).
6. Create a model line circle. On the options bar under Placement plane make sure you pick the reference lines plane, not only the current work plane even though it seems correctly matching the reference line plane. Make the circle with its center at the other end point of the ref. line. (Now the circle is hosted on the horizontal plane of the line. If you want, you can make the circle radius also parametric).
7. Create void extrusion by Pick lines or in the Edit Extrusion use Pick lines.
8. Select the circle and lock the padlock.
9. Finish sketch.
10. Flex.

Now parameters for the edges of the steel plate remain to be done. That will be my next struggle. Thanks for the formula list. I've seen it before, just forgot it.

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