How to center/Constraining a rectangular pattern to center of work surface part?

[mauribailey]

So I made this rectangular prism and then added a hole on one side (just picked any random location to start with).

I then made a rectangular pattern of 3x4 holes, each hole with a specific vertical and horizontal distance between their centers. The problem that I'm having now is that I want to be able to coincide the center of this pattern to the center of the work surface, that way if I wish to change the distance between the holes the pattern still remains centered to the work surface. Any advice?

[thenottakenname]

You may want to use construction lines and put a point in the center of your sketch. Then constrain that point to the center of your surface before you make the hole and do the pattern. 

[mauribailey]

Ok, I have made the necessary construction lines and constrained a point to the center of my surface. But what do I do next? Should I draw construction on my pattern and coincide the center to the point? (I do not think this is the best option because my pattern could change if I decide to add more holes to my pattern).

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[thenottakenname]

Here's a picture of what I mean. I've placed a point in the center of my sketch where the first hole is, and dimensioned the hole from it. The two location dimensions can be altered using parameters or changing them manually, then you change the pattern itself to place the rest of the holes where you want them. Hopefully this helps.

[SBix26]

If you want the ultimate flexibility, create four user parameters: QtyX, QtyY, SpacingX, & SpacingY.  Then set the first hole location from center to be SpacingX * (QtyX - 1 ul) / 2 ul & SpacingY * (QtyY - 1 ul) / 2 ul.  Set the pattern parameters to be the four user parameters created above.  Then you only have to change the four parameters to change your hole pattern and keep it centered.

Even better, instead of dimensioning the center point location, draw two construction lines, one from center of the left side, one from the center of the bottom side, each perpendicular to their respective sides, and joining where they intersect, which is now the center point.  That way the center remains the center no matter what size the face is, no re-calculating of dimensions required.

Sorry to not provide an illustration, but I'm away from my Inventor computer.

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Sam B
Inventor Pro 2020.0.1 | Windows 7 SP1
LinkedIn

[thenottakenname]

Well if we're going to get real fancy, may as well introduce iParts! In the most basic of terms, you convert a part to an iPart, then link in some of those custom-name parameters, and you can save multiple versions of the same part, but with different hole locations. It'll save you grief in the long run by not having to redo the hole locations you've already done. Worth looking into if you haven't already -- in for a penny, in for a pound right?

[JDMather]

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@mauribailey wrote:

... Any advice?

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My advice would be to Attach your *.ipt file here.

[mauribailey]

Here is an example of my *.ipt file. Nothing no complicated.

[johnsonshiue]

Hi! You could use Mid-Plane option in the Rect Pattern command. Simply change the hole distance to zero. The issue with your case is that there are 4 holes in a row. The starting occurrence will be the second one.

Many thanks!

[mauribailey]

Yes,  I was thinking about using the Mid-Plane option, but even this does have its limitations. If I was to have an odd number of holes in the vertical and horizontal direction (a square pattern that is not 2x2), I could use Mid-Plane tool and then coincide the center of my middle circle (in the pattern) with the center of my work surface, that way my entire pattern is always centered (no matter the distance between each hole or how many odd number of holes I add).

The problem seems to be with rectangular patterns that have even number of holes in either the vertical or horizontal direction. Invertor should have a tool that allows the user to center a pattern to a particular point or between two lines.

[johnsonshiue · Accepted solution]

Hi! I am not sure if this is totally related but take a look at the following thread. I think the OP was trying to do the same thing as you. There is a solution using iLogic. I proposed a simpler solution using parameter expression. Please take a look and see if it works for you.

https://forums.autodesk.com/t5/inventor-forum/problem-with-parameter-and-ilogic/td-p/8835687

Many thanks!