move origin in sketch 1

[altnickee]

Hi,

SW version 2007

in (extrude 1)I have a sketch in witch I want to relocate/move the origin from the left corner to the middle of the sketch.
I first tried the following: Click Edit sketch/in the sketch I click on the origin, and (in the existing relation box) I selected the coincident o, click delete on the keyboard, my sketch turns blue (under defined)
Second I place a centerline on which I want the new origin to move to.
I select the centerline (in the sketch) and the origin (in the Feature manager), but nothing happens?
I was expecting to see the selected entities in the property manager, so I can add the midpoint relation, to make my sketch black (fully defined) again.
Please help me how to move my origin in this sketch


Toolmaker

 

[MadMango]

Like this?

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[ctopher]

You can't move the origin, you have to move the sketch.

Chris
SolidWorks/PDMWorks 08 2.0
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[MadMango]

Riiiight, I had to add 2 centerline sketches and add relations to the origin, then remove the original relations of the sketches to the origin and add relations to the original sketch to the new centerlines using Symmetric relations. Catch all that?

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of Eng-Tips Forums?

 

[ctopher]

I have 2008, I can't send bakc the file for you.
Edit the first sketch, dim the arc, make both arcs equal.
Select the corner on the origin and remove the coincident.
Add a horiz centerline thru the center of the part mid-point to mid-point. Make the mid-point of this line coincident to the origin. Drag the arcs over and make center-points vertical to the origin.

Chris
SolidWorks/PDMWorks 08 2.0
AutoCAD 06
ctopher's home (updated 10-07-07)
ctopher's blog

 

[CorBlimeyLimey]

altnickee[/v],

Go to Tools > Options > System Options > General and select Auto-show PropertyManager.

 

[TheTick]

For some sketches, I'll draw fixed or constrained horizontal and vertical construction lines and used them as dimension datums/ origin. Sketch geometry is constrained such that the entire sketch can move just by dragging the vertex of the two datum lines.

For real thrills, do it all with no "vertical" or "horizontal" constraints, only parallel and perpendicular, and you can then also spin your sketch around 360°.

Honesty may be the best policy, but insanity is a better defense.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[altnickee]

Riiiight, I had to add 2 centerline sketches( one horizontal & one vertical?) and add relations to the origin(yes, but how?), then remove the original relations of the sketches to the origin and add relations to the original sketch to the new centerlines using Symmetric relations. Catch all that?
Please step by step, I understand what you are telling me, but don’t know the steps (or I am doing things wrong)


Toolmaker

 

[ctopher]

I have steps above.
If you right-mouse-click on a line, you can select mid and also mate as vert or horiz.

Chris
SolidWorks/PDMWorks 08 2.0
AutoCAD 06/08
ctopher's home (updated 10-07-07)

 

[altnickee]

I have 2008, I can't send bakc the file for you.
Edit the first sketch, dim the arc, make both arcs equal.(done)
Select the corner on the origin and remove the coincident.(done)
Add a horiz centerline thru the center of the part mid-point to mid-point.(done) Make the mid-point of this line coincident to the origin. (how?)Drag the arcs over and make center-points vertical to the origin.

Chris

Toolmaker

 

[altnickee]

altnickee[/v],

Go to Tools > Options > System Options > General and select Auto-show PropertyManager.(setting are like above)

cheers

Toolmaker

 

[TheTick]

Basically, you are anchoring your sketch using the two datum lines. The two datums lines should be constrained somehow (whatever the case calls for: dimensions to origin & datums, collinear w/ datums, etc.)

If you are using dimensions to constrain your datum lines, change the dimensions. If you are using constraints, delete the constraints and drag the datum lines around. If the rest of the sketch is constrained only to the datum lines, the whole sketch should move.

Practice with something simple.[/p] Start a sketch and draw and constrain two datum lines. Draw a simple shape and constrain its position to the datum lines. Change the constraints on the datum lines, move them, and watch.

 

[altnickee]

problem solved!!!

Thanks for the help

Toolmaker

 

[CorBlimeyLimey]

Are you holding the Ctrl key down when selecting the sketch elements?

Here's another example of how to re-position.

 

[ctopher]

Make the mid-point of this line coincident to the origin. (how?)

Right-mouse-click on the line, select mid-point, hold down Ctrl button, select origin, select coincident.

Chris
SolidWorks/PDMWorks 08 2.0
AutoCAD 06/08
ctopher's home (updated 10-07-07)