Centerline intersection dimensions

[EngJW]

Hello,

I have been learning Solidworks for a few days now and need help on the following:

I want to use the sweep function to make a tube with several bends. I would like to dimension to the intersection of the centerlines, but of course they go away once the bend radius is added to the path. Is there a standard method or a trick to do this?

Thank you
John Woodward

 

[mncad]

John,

Sketch the profile that you are wanting the tube to follow without the radii, then add the dimensions to the intersection points of the centerlines. After dimensioning, use the sketch fillet to create the radii that you need. The dimension will stay to the intersection point.

mncad

 

[TheTick]

To create an intersection point, select the two lines, and hit the "point" button in the sketch entities toolbar.

Intersection points look different than standard points. Appearance can be set in the options.

"Great ideas need landing gear as well as wings."--C. D. Jackson

http://www.EsoxRepublic.com

 

[EngJW]

Thanks very much!

John Woodward

 

[JNR]

Look up the help on "virtual sharp".

John Richards Sr. Mech. Engr.
Rockwell Collins Flight Dynamics

A hobbit's lifestyle sounds rather pleasant...... it's the hairy feet that turn me off.

 

[CorBlimeyLimey]

I agree with mncad's suggestion except, instead of clicking the end points of the line when dimensioning, click the line itself, then insert the radii. The dimension will remain at the original instersections. That's one less click per dimension.


CorBlimeyLimey, Barrie, Ontario.
I intend to live forever - so far, so good
faq559-863

 

[JNR]

One more thing...... If you dimension to the lines - as CBL says - before you insert the filets, it seems to be easier and cleaner.

One more thing (hey! I like Colombo...) It is always better practice to dimension to the lines anyway in my opinion - you have probably noticed by now I am not very opinionated, heh, heh This is really what you are trying to control with the dimension ie. the distance of the line from something, not where its end point happens to be at any given point in time. I put this squarely in the "design intent" concept.

I also like to use minium dimensioning and relationships and use them to force design intent. For example if I am making a square centered on the origin, I will create the rectangle, place a constuction line diagonal, make only enough lines equal to make it square, do a midpoint on the construction line and origin and add one dimension to one line. (That assumes the square will never be anything but a plain square, but you get the picture?) Note also that each line only needs one horizontal/vertical/perpendicular. I try to avoid or get rid of surplus relationships (and dimensions) and let the simple geometry control itself where appropriate. The more excess stuff the system has to compute, the slower things get. It might not seem much until you get to large parts and assemblies. Note that the system does not do this for you. Excess constraints do not necessarily mean an over constrained model. Those errors only (usually) pop up when there are conflicting constraints. But it is often easier to bebug if you get the error and have been careful about keeping down the excess.

John Richards Sr. Mech. Engr.
Rockwell Collins Flight Dynamics

A hobbit's lifestyle sounds rather pleasant...... it's the hairy feet that turn me off.