How do you dimension from a center point?

[cvriv.charles]

Say I have a simple object that looks like a ruler. I want a hole at the end that is dimensioned from the center of the ruler. How do you do that? I tried work planes and axis's but they fade out when I need them for this task. Please teach me. I only have so no much hair left. Thanks.

[JD Mather]

Attach the file(s) here.

[cvriv.charles]

Professor Mather, I figured out one way of doing it. I just thought there was an easier way of doing it.

 

I basically created a sketch on the face of the ruler. I had drawn a construction line at the center of the ruler. I then plotted a point using that construction line to dim from center. As said I just throught there would be a quicker way of doing it using the hole tool and maybe a workplane or axis instead of creating a sketch.

 

This is fine I guess. But if you know another way please do share:) Thanks.

[Denimoth]

I haven't had the time to really tinker with Inventor yet, but one way of doing what your asking is by using formulas in your dimensions. I can't save the file as a 2009 format (or I don't know how to if it can be done). Here's what I did.

 

1. In your hole sketch, add a dimension for the overall length of your "ruler". This will be a driven dimension, which is fine. In this case, the dimension is 12.

 

2. Add your hole (which you already did) then dimension from the edge of your part to center of hole.

 

3. Edit this new dimension, and shift-click on the 12" dimension, which Inventor has identified as d14. If you want to specify a distance from the middle of the part to the hole, type ( d14 / 2 ) - 5.5. Since d14 is equal to 12, the math is 12/2-5.5 = 6-5.5 = 0.5". In other words, you're telling inventor to take the value of dimension line d14 (which is 12"), divide it by half to find your middle point, then subtract that value by 5.5. (edit: the d14 is a specific tag for the 12" dimension. The tag name will always be different for every new dimension you make, thus why you shift click on your reference dimension so that you can extract that dimension's specific tag identifier).

 

Edit: I changed and added to my explanations. Wasn't very well written and left the possibility for someone else to make errors trying to follow the steps.

[shift1313]

i wrote a reply then my browser crashed!

 

One way you could do this is by centering your shape around the origin. Do this by drawing your rectangle then adding a vertical line that snaps to the center points of your long edges. Make this vertical line a Center-line.

 

Place a coincident constraint with the origin and the center point on this center-line. Then add your dimensions by selecting the opposing sides. For instance you select the two 1" vertical lines to create your 12" dimension.

 

I added the hole to the first sketch. I gave it a horizontal constraint by selecting the origin and the center point of the circle.

 

For the horizontal distance(since you were asking about this) i added a dimension but created an equation(just like denimoth mentioned). When the box shows up and your value is highlighted, you can either type the name of the other dimensions or click on them. in my case the 12" dimension was d0 so my equation was (d0/2)-1. I wouldnt typically dimension that hole to the center point but this is how you wanted to do it. The diameter is used the 1" dimensions /2. so d1/2.

 

Here are two screen shots to show you constraints and dimensions.

[cvriv.charles]

Awesome will try that out. Very cool. Thanks guys:)

[kencaz]

You can also center constrain your rectangles using a vertical and horizontal constraint as such:

 

 

KC

[stevsmith]

You can also center constrain your rectangles using a vertical and horizontal constraint as such:

 

[ATTACH]17804[/ATTACH]

 

KC

 

Nice tip man!

[cvriv.charles]

OMG I love the vert/ horz constraint method! I was using those for lines only:( But you can use them to constrain all kinds of stuff to mids points etc. I was dim'ing everything,...