Move Sketches 2

[SBaugh]

You would think this would be self explanatory, but I am having a heck of a time moving sketch entities.

I have a base sketch that I have remove all the dimensions making it defined so it can be moved. When I select all the sketch entities and click Move/Sketch Entities it has all the sketch lines pre-defined. I want to use the From\To option. I made a special construction line to move from one point to another. I click the first point and I get the yellow globe... I cannot go any further, every point, edge line, out in space that I select I just seem to re-select the start point and the sketch never moves.

Anyone else seeing this?


The help reads:

From/To. Adds a Base point to set a Start point and a destination.

The image that is provided just shows the user placing the entities where they want it in space from one point to another... not working here!

VAR is not any help today when calling in, because they never pick up the phone.

Regards,

Scott Baugh, CSWP
Berry Plastics
Cad Admin\Design Engineer

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[SBaugh]

Never mind I found a relationship that was keeping me from moving the sketch profile...


Sure would be nice if the Command gave a reason why a user could not move the sketch. Wasted about 20 minutes trying to figure out why it wouldn't move.

I have found many commands that just don't give enough or any information as to why they will not complete the task.

Regards,

Scott Baugh, CSWP
Berry Plastics
Cad Admin\Design Engineer

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[ctopher]

Or try "Tools/Sketch Tools/Modify".

Chris
SolidWorks 10 SP4.0
ctopher's home
SolidWorks Legion

 

[SBaugh]

Problem with Modify is that its not specific enough... i just needed to move the whole profile up vertically without changing anything. Modify was just more trouble than it was worth. Modify is great for the eyeball close sketch stuff... I never use it for anything I need something specific.

Move sketch entities still didn't work, I had to copy the sketch and remove the original sketch... which means everything in my tree is going to fail, surfacing... everything associated to the Base sketch profile will fail now.


Thanks Solidworks for making Move\Sketches so simple! This will now put me hours behind schedule and the file is due tomorrow.

Regards,

Scott Baugh, CSWP
Berry Plastics
Cad Admin\Design Engineer

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[rgrayclamps]

Hi, SBaugh:

Moving sketches in SW is very easy.

1) Window select all entities you want to move;
2) Ctrl select a point (from);
3) Release ctrl key;
4) Drag N drop to target point;

Good Luck!

Alex

 

[rgrayclamps]

Hi, SBaugh:

I tried "Move Sketch Entities" command. I duplicated your finding.

If you try the method I use, you will be able to move any of sketch entities around precisely.

Best regards,

Alex

 

[Nella95]

Sometimes if you're dealing with an imported AutoCAD or *.dxf - you have to 'copy' instead of 'move' - then delete the original.

 

[TheTick]

Never mind I found a relationship that was keeping me from moving...

Been there!

 

[SBaugh]

Yes holding Ctrl worked... would have been nice if the help actually listed that as the requirement to move the sketch.

From the help file 2010:


Move or Copy Sketch Entities
To move or copy entities:

In sketch mode:

Click Move Entities (Sketch toolbar) or Tools, Sketch Tools, Move.


- or -

Click Copy Entities (Sketch toolbar) or Tools, Sketch Tools, Copy.


Dimensions are moved or copied to the new location with the entities. Relations are moved or copied only if you select Keep relations.



In the PropertyManager, under Entities to Move or Entities to Copy:

Select sketch entities for Sketch item or annotations.

Select Keep relations to maintain relations between sketch entities. When cleared, relations are broken only between selected entities and those that are not selected; relations among the selected entities are maintained.

Under Parameters:


Sketch Type
Instructions for modifying parameters

2D Sketch

3D Sketch On Plane
Do one of the following:

Select From/To, click Start point to set a Base point , and then drag to position the sketch entities.

Select X/Y and set values for Delta X and Delta Y to position the sketch entities.

Click Repeat to modify the position of the sketch entities again by the same distance.



That really needs to be updated... holding that one button did not occur to me and would have saved me hours worth of work.

Scott Baugh, CSWP
Berry Plastics
Cad Admin\Design Engineer

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[rstupplebeen]

Sketch blocks may also come in handy.

Rob Stupplebeen

 

[StefanHamminga]

Very simple trick i use to find unwanted references is just to overdefine the sketch by adding a dimension that would move your entities in the same way that you would by dragging. When it gets turned to 'driven' right away set it to driving again. After that just hit the solution generator button and see what rolls out, much quicker than checking each entity.


Stefan Hamminga
EngIT Solutions
CSWP/Mechanical designer
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