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Has Inventor a "divide" command, similar to ACAD ?
(had to go look in acad to see what the Divide command did...it's been a
while) Here's one way to get that functionality in an Inventor sketch....
Lets say you need a 26" line, divided into 6 equal segments:
-Create a construction line, and dimension it to the 26" overall length you
need. Check in the parameters dialog and make a note of the parameter
that's assigned to that dimension. In the screencap, mine is d1.
-Now place a sketch point at the beginning of the line.
-Invoke the Rectangular Pattern command. Choose the sketch point for the
geometry, and the construction line for the direction. Make sure the
preview has the array going in the right direction.
-Enter the number of points you want, which would be seven (the number of
segments you want to divide the line into plus one).
-For the spacing, enter in d1/6
This will get you a series of points that effectively divide the line into
segments. There are other ways to do this as well, but this is one of the
quickest and most versatile for times when you need a lot of little
segments.. Everything stays intelligent, and can easily be manipulated as
needed. This method has lots of useful variations. I used it this week to
place evenly spaced rivet holes in a sheet metal piece. The holes had to be
3/4" spacing, with as many as could fit on the length of the part in a
centered pattern. I had several pieces of varying lengths to model. Here's
what I did:
-Sketch a construction line representing the entire array as above.
Constrain it's centerpoint to the middle of the part so that the line always
-Dimension the line, and for a dimension value, enter .75 * X. Play with
the value of X until the optimal fit is achieved. The value you settle on
for X will be the number of segments the line is divided into, so the number
of points for your array will be X + 1.
Here is another method.
Dimension the line you want to divide.
Place a point at the end of the line.
Do a rectangular pattern of the point and to enter the length of the line simply click on the dimension.
Expand the rectangular pattern dialog box and select fitted.
If you later change the dimension the divisions will update.
There are other methods as well. I prefer to NOT pattern sketch entities in most instances and rather pattern features. The Rectangular Pattern-feature tool is misnamed as you can pattern along feature shapes.