Best way to sketch centered rectangle?

[valbotany]

Sorry for the ultra basic question.  But I ask it partly to make sure I am "getting" the Inventor style of approach to things.  I am using Inventor 2012 and want to know the best general approach to centering things like rectangles.  I know newer Inventors have a different rectangle tool for this.  But can anyone tell me the ideal approach to placing your first geometry such that it is centered in the screen?

For example, is it best to draw a quadrant of your rectangle, make 2 centerlines, do 2 mirror operations, and then delete surplus lines?  Or would it be better to somehow locate the midpoints of your two major lines onto the two axis and then fill in the rest after?  Just curious what the smartest approach to this is in Inventor.  After all, possibly the majority of parts start with operations like this.

[mdavis22569]

Simple ....4 dim's

do 2 overall's ..then project center point ..then do dims' that are 1/2 of the overall ..

this then will leave you the planes to use for constraints

[JDMather]

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@mdavis22569 wrote:

Simple ....4 dim's

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No, no, no............

There is already a Center Point Rectangle tool.  Only 2 dimensions are required.

...even before the Center Point Rectangle tool was added to Inventor - only 2 dimensions were required to dimension a rectangle.

Pg10

http://home.pct.edu/~jmather/SkillsUSA%20University.pdf

Mirror?  Delete surplus lines?

Why would you ever have surplus lines to delete?

Use Construcion lines when appropriate (I use lots of 'em).

If you look around the world, either at man-made objects or nature, you will generally see lots of symmetry.

Make use of obvious symmetry in your designs about the origin.

If there is no obvious symmetry, or you need (for some odd reason) to specify a manufacturing origin in your part - then place the lower left corner at the origin (geometry in the positive octant).

Those are the two rules I use.

Pattern features rather than sketches if possible (and logically appropriate).

[mcgyvr]

http://blogs.rand.com/manufacturing/2010/12/inventor-add-in-center-point-rectangle.html

[JDMather]

You mean it wasn't added till r2013? 

Well load the add-in and don't look back. 

[mdavis22569]

I showed this way ..since he was in 2012 ..not 2014/15

[mcgyvr]

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@Anonymous wrote:

You mean it wasn't added till r2013? 

Well load the add-in and don't look back. 

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yep wasn't added till 2013..

[JDMather]

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@mdavis22569 wrote:
I showed this way ..since he was in 2012 ..

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Man that is hard to believe, I thought we had it at least 2 yrs earlier.  I guess I was thinking of the add-in.

No wonder everyone went to another SoftWare.

[mdavis22569]

I joined a new company in May ..and they are on 2012 here ... and I'm going NUTS, otherwise I would have done the rectangle too .. But one a good note for me, I did find out that we're going to 2015 at the beginning of the year.

[JDMather]

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@mdavis22569 wrote:
I joined a new company in May ..and they are on 2012 here ... and I'm going NUTS,....

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Download the Add-in that mcgvr linked above.

[Anonymous · Accepted solution]

Draw rectangle and dimension length & width, put a diagonal construction line between opposite corners, then constrain the middle of the diagonal to the origin.

[cmharb]

We simply use the Horizontal and Verticle Constraints on the mid point of the line to the centre point in the sketch.

And the sketch is centured needing only 2 constraints and 2 dims. If you need a square use the Equal constraint on two perpendicular lines.

[JDMather]

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@cmharb wrote:

We simply use the Horizontal and Vertical Constraints on the mid point of the line to the centre point in the sketch.

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I recommend not doing it that way.  Diagonal line (in old versions) is more robust technique (and in my opinion, easier).

I demontsrate two reasons not to do it that way in paper linked above. (and there are other reasons)

[cmharb]

it is out standard to do it this way.

In your examples (19,20,21) they are not rectangles.

In 19 the rectangle would be extruded then the radii added.

in 20 the rectangle would be extruded then the extra bit added and extruded.

[valbotany]

mdavis22569

Do you mean to go into the Parameters and create new mathematical relationship assignments, or is there a way to achieve this implicitly in the sketch?

[mdavis22569]

Here is an example ipt sketch

[JDMather]

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@valbotany wrote:

@mdavis22569

.... is there a way to achieve this implicitly in the sketch?

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When entering the "half" dimension simply click on the "whole" dimension and /2.

You do not need to go into Parameters.