Rotating Sketch entities 1

[gatz]

I do not understand how to Rotate Sketch entities to align with a construction line. Maybe this is something simple, but it escapes me.
For instance... if an Open Sketch has 2 circles; one of which is at the Origin. The other is some distance away in X+, Y-
A construction line is drawn at X+ Hor; (although there are common situations where a construction line at any angle to "normal" x-y may be needed.)

If I use Tools, Sketch Tools, Rotate, select the Center of the circle that's not at the Origin,
then ?????? what ???

If I attempt to Rotate the 2nd circle about the Origin, and as it approaches the Hor line, it appears that it is "snapping" to the line. When I click OK, it's 270deg from previous position.

I've also tried changing the dimensions to "Driven". Tried using a centline distance dimension that was not driven....
etc, etc

http://img.photobucket.com/albums/v630/Gatz/RotateSketchQ.jpg

There must be an easy way to do this.
As an old AutoCad user, this operation is very basic and intuitive.

 

[JMirisola]

Select the center of the circle in question, hold down the ctrl key and select the construction line, then select coincident from the relationship choices in the feature manager.

Jeff Mirisola, CSWP

http://designsmarter.typepad.com/jeffs_blog

Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M

 

[CorBlimeyLimey]

You don't need to use the Rotate tool.
The Ø1.000" circle is not at the origin. If it was, it would be coloured black.
Delete all but the 1.000, .5625 and 2.3654 dimensions.
Then just grab the .5625 circle centre and drag it onto the CL. (or do as Jeff said to force a constraint).

Can you post an image of the 270° misalignment?

 

[gatz]

Cor,
Here's the Sketch when I've attempted to grab the center of the .5625 circle and Drag it to the Hor construct line. (Using the Tools, Sketch Tools, Rotate command)
It "snaps" to the line, but then for whatever reason, it wants to displace the cirlce 270deg from the present position. And the angle box reflects that. There's also a mouse icon on the screen with the OK-right button click which "Print Screen" does not pick up.

http://img.photobucket.com/albums/v630/Gatz/RotateSketchQ_2.jpg

Note that the 1" circle IS at the Origin (black now), but the only thing done differently was to change what were Driven dimensions to un-Driven.....which is another thing I don't quite get. How is it that the circle becomes defined, when the dimensions' state is the only thing changed.

The reason there are 0.000 dimensions is because I had previouly moved both circles from an arbitrary location such that the 1" circle was moved to the origin.

This whole excercise was to show my son how to translate dimensions of features from those gathered from a CMM, and construct a model with the center of a given bore diameter (1") as an Origin, with the other features relative to it and the .5625 hole being Horizontal (X+)

 

[CorBlimeyLimey]

"How is it that the circle becomes defined, when the dimensions' state is the only thing changed."
Because it's the dimensions which are constraining the position of the circle. Making the Dimensions Driven is like suppressing the constraint ... or suppressing a Driving dimension.

 

[gatz]

OK, maybe I didn't make the example very clear as to what I'm trying to do.

I have taken x,y coordinates off a CMM and made a sketch showing those points/features.

Because the CMM uses an origin NOT on the part and it's X-axis is NOT in line with any given part feature and because it did not have the software that would transpose/translate those dimensions to some known feature, the attempt was to do it within a SW sketch.

Those entities needed to make an Extrusion or those needed to make Cuts, or those needed for relative placement of Points would then be made available.

In the Help for Rotate, it says to drag one of the Handles on the Rotate Point Defined icon. Then what????????
It only moves a random value...

I cannot see how to get the center of the .5625 hole to be lined up horizontally in the X + axis (whatever that angle might be...it doesn' really matter) and with all the other sketch entities moved the same relative amount about the center of the 1" diameter (the sketch origin)
Once this is done, I can model up the part with the 1" diameter "hole" at the origin and the .5625 diameter on the X horizontal line.

JMirasola, I had also tried to get the center of the .5625 circle to "Add Relation" Coincident with the contruction line, but SW does not allow that whilst in the Rotate operation.

Hopefully, this pic will better explain the situation.
Gatz

http://img.photobucket.com/albums/v630/Gatz/rotatesketchq_6.jpg

 

[CorBlimeyLimey]

Select all the entities and turn them into a block. Select the centre of the 1" circle as the Insertion Point.

Once the block is created, drag the centre of the 1" circle onto the origin.

Then drag the .5625" circle onto the horizontal.

 

[CorBlimeyLimey]

If you still want to use the Move/Copy and Rotate functions;

http://screencast.com/t/bZaoYZtMwaY

 

[gatz]

Cor,
Thanks so much for the help.
I followed the "Block" entities routine and that works fine.
(I checked the geometry, and all was OK)

The short video was even more helpful, and shows another way to get the incremental angle move.

Gatz