Why doesn't Automatic Relation work between Sketch Points? 1

[brengine]

Start a new sketch and insert a sketch point. Now, start to draw a line, but before you click to start the line move until the horizontal dotted line (i.e. Inferencing Line) shows up between your cursor and the sketch point, now click to start the line. Notice that if you draw the line horizontally, you'll get a Coincident relationship between the line and the existing point, but if you draw the line in any other direction...there will be no relationship created between the line and the point.

So the question is, if I had a horizontal dotted (Inferencing) line between the Sketch Point and the starting point of the line, then why isn't there a horizontal relationship created? I saw the little relation box with the white background pop up next to the cursur saying that the place point was in fact horizontal to the Sketch Point, but no Relation was created.

From further experimenting, I found that only when the little relation box next to the cursor had a yellow background...would an Automatic relation be created. But I could only get the yellow box if sketching line to line, or Horizontal/Vertcal with a sketch point, or putting a sketch point on the line.

To take this one step further, go to put another sketch point in. The only time an Automatic Relation (i.e. yellow background box next to cursor) will show up is if you are actually going to place the Sketch Point on the line or one of it's endpoints.

Any idea how to create an Automatic Relation for one of these Sketch Points if I don't want to place it on the line?

Thanks,
Ken

 

[CorBlimeyLimey]

Sorry, I don't know how to force the automatic relation of sketch points. Even if I did know, I probably would not use it.

I prefer to use actual geometry (lines & arcs) to make the constraints. I find they are more obvious & easier to see & understand when troubleshooting or investigating a sketch. But that's just personal preference.


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[brengine]

CBL,

I do agree and recommend your method as well, but not everyone here feels that way.

Also, holding down the [Ctrl] key while sketching turns Automatic Relations off until the [Ctrl] key is released. So why not let the User choose whether to not to add the Relation? There's already the Inferencing Line there as well as the possible Automatic Relation(s) with the white background.

Still wondering,
Ken

 

[ctopher]

What sort of relations do you want? I'm not clear.
Can you show us a screen shot of what you see?

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[brengine]

A Horizontal or Vertical relation between the sketch points as the dotted (Inferencing) lines implied would be there.

Ken

 

[smcadman]

If I draw the POINT first, then a LINE can inference it and create a coincident sketch relation. But if you draw the LINE first, the POINT will inference the line, but no sketch relation will occur. You will get a white inference box instead of the yellow relationship box (see screenshot).

http://img297.imageshack.us/img297/4461/inferenceandrelation2ym.jpg

You will have to manually create the relations you want. Incidentally, the same is true for a circle. Draw a line, then move over horizontally and start the circle. The center point of the circle will inference a line, but not create an automatic relation.

Flores
SW06 SP3.0

 

[dezignstuff]

The dotted "inference" lines do not create relations. This is one of the questions that always shows up on the various tests including CSWP. The only times relations are actually created are when you can see the "coincident" or "midpoint" symbols next to the cursor.

There is one exception to this. When you draw a line such that both endpoints pick up the same inference to another sketch point or the origin, you will get a coincident relation between the point and the line.

To my knowledge the only relations you can get automatically with a 2D sketch point are coincident and midpoint. 3D sketch can get others such as on surface. Horizontal and Vertical relations are always manual for sketch points.

matt