Say I have those 4 elements selected (2 centers of circle, 2 edges of square). I now want the circles to be in equal distance from the edges. Isn't there a simple function for it so I won't have to do any calculations?

-Val

Say I have those 4 elements selected (2 centers of circle, 2 edges of square). I now want the circles to be in equal distance from the edges. Isn't there a simple function for it so I won't have to do any calculations?

-Val

@Krzys That would mean they would be in equal distance to each other, I want equal distance from two edges

@Rob This works, thanks!

Valery Volkov wrote:

@Krzys That would mean they would be in equal distance to each other, I want equal distance from two edges

@Rob This works, thanks!

As Kryzs stated, it's the same thing as what Mr. Edwards posted.

The sketch mirror operation creates symmetry and equal mates relations.

Also, in your OP image, you have two dimensions for the circles that's the same value.

This is consider poor design intent practice.

Paramount would be to add an equal mate relation, if you didn't need the symmetry.

Optimally, would be to use Hole Wizard (and in the Hole Wizard sketch, the points would be mirrored).

Kevin

Because your square is vertical and horizontal, you can simply create a vertical relationship between the two holes' centers.

If it was not ortholinear, the symmetry would still work. A very easy way to extend this to all circumstance is to create two construction lines from the near edge to each circle center, and parallel to the other edge, and make those construction lines equal.

Hello,

Since your sketch is orthogonal, you can do this with one line at 45° and an edge dim and a sketch mirror:

This is in Hole Wizard and since Hole Wizard only uses points, construction geometry doesn't have to be construction type.

Also, you can do this with two dimensions and set one equal to the other:

This makes the design intent more evident as a dim with an equation (with a red uppercase Sigma) isn't supposed to be edited directly, but driven by other parameters.

Note, too, with Hole Wizard, the sketch mirror only creates a symmetry relation since an equal relation for points is nonsensical.

Kevin

Hello,

Create a horizontal (or vertical) edge midpoint to midpoint .

Create a midpoint line at the midpoint of the first line.

Mirror the second line about the the first line.

Add the hole entities to the four line endpoints.

The main benefit of this method is that the symmetry is in the lines and not in the hole entities.

This permits being able to place any hole type on any endpoint and still maintain alignment:

The right hole is related Equal to the left hole.

The right slot is related Equal Slot to the left slot.

The width of the left slot is equated to the left hole's diameter dimension.

This works in a Hole Wizard sketch, too, except it's not required that these lines be of construction.

[Not true. I forgot that's there's a point at the middle, so for HW, the separate sketch workflow is required for this method.]

I'll also recommend that the hole entities operation be separate from the extrude operation for creating the square.

Kevin

Hello,

Another method that puts the symmetry in the sketch entities and not the hole entities is to use a center rectangle:

If this method is used for non-Hole Wizard holes, then all sketch entities are to be of construction.

If this method is used for Hole Wizard holes, then all sketch entities can be as created, however since the center rectangle has a point entity with relations, this point will create a hole in Hole Wizard.

To get around this, the hole locating sketch must a sketch (absorbed or unabsorbed) created before the Hole Wizard operation. It has to be visible, too.

The Hole Wizard uses the face of the extruded square for point placement, but the points are snapped to the corners of the rectangles in the referenced sketch:

Like the previous method, the hole type can be varied, but with each Hole Wizard type/size, a separate Hole Wizard operation is required. Multiple Hole Wizard operations can be created referencing the same sketch as often as is necessary to create the required holes:

When done, hide the reference sketch:

Kevin

How about symmetric?