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Mechanical Engineering Home >Info: Useful Links > ProE > Align

Why do I need to align and dimension? Shouldn't Pro/E just know automatically how big I want things?

No. Pro/E assumes a lot about sketches you make, but it was only written by a human, and cannot predict what size you want a sketch to be. Besides, imagine how annoying it would be if Pro/E only used the sketch you drew on the screen- you would have to have nearly perfect mouse control just to draw a cube, never mind a complicated section.

What's the difference between aligning and dimensioning?

Dimensions tell Pro/E something about the relationship of two features. They either specify a distance, an angle, or a radius/diameter. Aligns tell Pro/E to "glue" one line to another.

Don't I have to align lines to datum planes to make them parallel?

No. This confusion is caused by poor choice of vocabulary on the part of the programmers. Align in this sense does not mean "make parallel to." It means "make the distance between these two things zero." When used, it makes two features coincident.

If a line you have drawn in the Sketch mode is close to a datum plane (or supposed to be on it), you need to align the line and the datum plane. If a line is farther away, then Pro/E will not let you align it, so you must dimension it.

How do I know Pro/E will make corners square and my lines parallel to the datum planes?

The simple answer to this is: "You just do." Pro/E is very good at assuming things about your sketch. If you drew it reasonably parallel to a datum plane and don't tell Pro/E otherwise, then they will be made parallel when you regenerate.

Suppose I want a line at an angle to a datum plane... what do I do then?

Simple: draw the line at roughly the angle you want, then dimension the line at an angle to the datum plane. To do this, choose the dimension menu item, click on the middle of the line with the left mouse button, then on the datum plane with the left mouse button, then with the middle button where you want the dimension to appear. This will then appear as an angular dimension which can then be modified.

What else do I have to align?

• Always align centerlines to datum planes, or explicitly dimension them at a certain distance or angle away. Since centerlines are always infinitely long, you don't have to tell Pro/E how long the centerline is.
• If you want a point on your sketch to fall at the intersection of two other features (say a datum plane and a circle), align the point to each item separately: click on the point, then on the first item, then click on the point again, then on the second item. This creates two separate aligns for that point.
• Center points of circles need to be aligned or dimensioned.

Anything else I should know about?

Tons, but it is far easier to learn them by using Pro/E than reading a web page. A good rule of thumb to use is this equation:

N = 2P - L + 3C - A

N is the number of aligns/dimensions you need. P is the number of points on the sketch. L is the number of lines on the sketch that are parallel to the datum planes, C is the number of circles and A is the number of arcs on the sketch.

Yes, you probably don't want another equation. You may not even use this equation, but going through how it was derived could show you a better mental model for figuring out how many dimensions and aligns you need.

• Think of a point lying on a plane. It needs two dimensions (or aligns) to completely specify its location. Hence the 2P.
  
  
  
• Think of a straight line at some arbitrary angle. It has two points, so it has N=2*2=4. Thus you need 4 dimensions (or aligns) to completely specify the line in space.
  
  
  
• Think of a line parallel to a datum plane. If we completely specify the location of one endpoint, we have already specified one degree of freedom of the other endpoint (since Pro/E will assume that the line is parallel to the datum plane.) Thus, we have N=2*2 - 1 = 3. The other dimension necessary is the length of the line.
  
  
  
• Now think of a circle. We need to specify the location of the center point (2 dimensions/aligns needed), and either the radius or diameter (1 dimension.) Thus each circle takes 3 dimensions or aligns to be completely constrained.
  
  
  
• Finally, consider an arc. It's like a straight line, but it has the qualities of a circle. If we pretend it's both, we get 2 endpoints needing 2 dimensions each, a center point needing 2 dimensions, and a radius needing one. Since the endpoints of the circle are accounted for in the 2P term of our equation, we need only add the three dimensions necessary for the center and radius of the arc. However, once we have specified one endpoint, the radius, and center of the arc, we only need one more dimension to completely specify the arc (the other is implicitly specified by the rest of the arc), so we subtract one degree of freedom for each arc in the sketch.
  
  

Basically, you need to specify the dimensions so that Pro/E can find every point on the sketch.

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