I need to stretch this sketch to the corners of the rectangle. I have lots of these in different sizes and styles. They are scanned from Jpegs. So, I don't want to spend lots of time to define every line, arc etc.. Is there a way to stretch them EVENLY to the right position?
thanks.
Unfortunately SW is very limited with regards to sketch manipulation other than actually editing the sketch. You can't mirror, stretch, or bend a sketch. If you are using auto-trace on a sketch picture it will probably be easier to scale the picture first, then trace it.
If that is not an option, you'll need to create a feature using your sketch and then scale the resulting body. Hopefully the sketch consists of non-intersecting contours. You can try to just extrude the sketch as a surface, then use the scale feature on the resulting surface body, then start a new sketch and convert the edges of the scaled body. In order to figure out the scale value I think you'll need to calculate it manually by measuring the source and destination dimensions.
Hi Jamil. Thanks for reply. Scaling will not work because I need to scale in different ratio on X and Y directions. I saved as DWG and was able to do it in Draftsight.
In newer versions of solidWorks you can scale by different amounts in each direction. I am not sure when they added that ability but as of 2014 you can do it. But I'm glad you found a solution anyway.
I use 2014 SP 3 and I am not able to scale in different lengths.Perhaps they added in later service packs. That would realy help if you are able to do it because working between 2 programs take a lot of time.
Just to be clear, I am talking about the Scale feature that is applied to bodies, not the Scale tool for scaling sketch entities. So if you can convert your sketch to a body or bodies, for example by doing a surface extrude, then you can scale those bodies unevenly. You just need to uncheck the "Uniform scaling" box and then you can enter a different scale value for X, Y and Z directions.
Sey Tay wrote:
Hi Jamil. Thanks for reply. Scaling will not work because I need to scale in different ratio on X and Y directions. I saved as DWG and was able to do it in Draftsight.
sometimes it takes more than one program to get what you need, so just resave the DWG and reopen them in SW then model your parts.
You are somewhat fortunate that the shape you are scaling consists only of lines. This opens up more possibilities.
You could define the spacing of the segments in a relative manner, e.g. as a fraction of the overall length/width. Then the spacing in each direction will scale with the overall length. You might also exploit equal length and symmetry constraints and constriction geometry.
Sketch blocks are scalable, but only overall and not in multiple directions.
You could possibly make construction sketches for guide lines in X and Y directions. Then a 3rd sketch can just lay on the guide lines, while the X and Y sketches are independently scales.
Surface bodies can be scaled in multiple directions. Make a surface extrude of your sketch, scale the surface, and then use the surface edges to create final.
As others have noted sketch scaling in SW is not as robust as solid scaling. The best I can come up with is to do it in two steps, one for each direction. Use "Sketch Tools/Scale. . ." to scale the sketch in the largest direction. Then create a plane with the appropriate orientation and angle to scale down in the other direction by converting entities into a new sketch.
Here Sketch1 started as a 1" square centered on the origin. To scale it 2 in the X direction and 1.5 in the Y direction, I used the Scale tool to make it a 2" square (as shown). Then I made sketch 2 on the right plane to get the angle for the plane that Sketch3 will be on. The 1.5" dim. in Sketch2 would vary, depending on the desired scale and the size of the original sketch. Open a sketch on the new plane, select Sketch1, "Convert Entities" and you're done. If you need the sketch back on the original plane, you can either make a derived sketch, or if having an undefined sketch is OK, delete all the relations and change the sketch plane to the desired one. You could delete the "construction" sketches and plane too if you want, that's what I did in the second example, excepting that I left the original (in red) for reference.
The method is a bit round-a-bout, but not really that difficult or time consuming, it harkens back to the pencil and paper days of pulling an auxiliary view or ductwork pattern. If I had a lot to do I would probably get Draftsight or something and do my 2D manipulation there, but for occasional odds and ends it's an effective method.
Interesting approach Erik. But my sketches come from some photos. Undefined and very complex to control. all those lines and arcs will not proportionally scaled to each other. Only way is to be able to convert them to blocks and define X,Y values separately but that does not seem to be possible in Solidworks.
Can you post an example we can play with?
Hi Erik,
Take a look at the attached Solidworks file. Please try to scale small boc in the exact corners of big box. You can use any other program. Obviously, It is very complex and time consuming to create this from scratch.
no file put up!
I think the way you are doing it using Drafsight may be the easiest.
Is this what you are looking for. Sorry it took a bit, I was out this morning. The time spent was about 15 minutes download to reply.
Hi Erik. Yes this is what I needed. I have to read you previous post more carefully to understand how you did it.
thanks.
Are you able to extent in X and Y directions independently?
Yes you can scale each direction independently.
I was reminded of making an "elliptical" spiral by projecting a true (circular) spiral onto a plane at an angle to it. The way a circle is elliptical when viewed at an angle. I first though "Ah, just do that twice, once for each direction" but then I realized that the method will not work to stretch a shape, only compress it. It occurred to me that the if the sketch is being scaled by different amounts in each direction the sketch scale tool could be used for the larger direction and the "projected on a plane" for the smaller.
I think it will be apparent how Sketch2 is set up to fix the angled plane at the correct angle when you have a look and consider what's going on.
I attached a PDF with a bunch of screen shots and brief explanations. See if any of it makes any sense, and let me know what isn't clear.
Thanks Erik,
This PDF explains what I need.
you can make blocks in SW
You create blocks from single or multiple sketch entities.
Blocks enable you to:
| Make Block | Convert sketch entities to blocks. A Block is identified by |
| Edit Block |
|
| Insert Block | Create multiple instances of existing blocks or browse for blocks to retrieve blocks in parts, assemblies, or blocks. |
| Add/Remove | Adds or removes sketch entities from a block. |
| Rebuild | Rebuilds and updates parent sketches by the block. |
| Save Block | Saves and adds an .sldblk extension. |
| Explode Block | Dissolves the block.Exploding one instance of a block only affects that instance of the block. |
| Belt/Chain | Creates continuous tangent lines and arcs to represent the belt or chain path. |
If you use another block with convert entities, the resulting geometry is not associative to the original geometry.
Related reference
Search 'Blocks in Parts and Assemblies' in the SOLIDWORKS Knowledge Base.
As others have noted sketch scaling in SW is not as robust as solid scaling. The best I can come up with is to do it in two steps, one for each direction. Use "Sketch Tools/Scale. . ." to scale the sketch in the largest direction. Then create a plane with the appropriate orientation and angle to scale down in the other direction by converting entities into a new sketch.
Here Sketch1 started as a 1" square centered on the origin. To scale it 2 in the X direction and 1.5 in the Y direction, I used the Scale tool to make it a 2" square (as shown). Then I made sketch 2 on the right plane to get the angle for the plane that Sketch3 will be on. The 1.5" dim. in Sketch2 would vary, depending on the desired scale and the size of the original sketch. Open a sketch on the new plane, select Sketch1, "Convert Entities" and you're done. If you need the sketch back on the original plane, you can either make a derived sketch, or if having an undefined sketch is OK, delete all the relations and change the sketch plane to the desired one. You could delete the "construction" sketches and plane too if you want, that's what I did in the second example, excepting that I left the original (in red) for reference.
The method is a bit round-a-bout, but not really that difficult or time consuming, it harkens back to the pencil and paper days of pulling an auxiliary view or ductwork pattern. If I had a lot to do I would probably get Draftsight or something and do my 2D manipulation there, but for occasional odds and ends it's an effective method.