I have two questions here.
1. How many relations are possible at one time to make the sketch below ?. I ask because I'm trying to figure out the fastest way to make the symmetrical parts of the sketch with out dimensioning each part ?
2. I'd like to save the sketch below as a file, (after it's finished of course) to then later paste or apply on a model at a later time, to then boss or cut an extrusion.
Not sure how to do this or if it's possible ?
Thank you. Frank
I would fully define one of the four cuts and use a pattern.
As for the sketch you can draw it on a new part and save it, when you need just access it and copy the sketch.
Jean G.
Jean Giacomoni wrote:
I would fully define one of the four cuts and use a pattern.
As for the sketch you can draw it on a new part and save it, when you need just access it and copy the sketch.
Jean G.
You can also save the Part with just the sketch, then insert that Part into another Part. Positioning the sketch might get a little tricky in the new Part, but it can be done. I've used this approach a few times to sketch a concrete profile, then insert the sketch Part into my rebar Parts and reference it to keep clearance. That way if the rebar size changes the rebar will update with it.
Also a good method, I guess the approach depends on the type of part he wishes to make the cut, if it is easy or not to locate the cut.
To save a "sketch" as a separate file, make it a block then save out the block.
Ensure the sketch is highlighted in the feature tree. Then click File, Save As. Change the file type to SLDLFP (Library Feature Part). You will notice the sketch will now have a "L" over top of the symbol in the tree. Once it's been saved you will notice some additional folders in the tree (References, and Dimensions). Add and locating dimension to the correct dimensions folder.
You can add this to a design library location to easily drag it into a part you are working on. It doesn't have to be in a design library folder though.
Lastly you can also have multiple sketches/features as part of a SLDLFP. For example you could have a sketch and extrude.
Hello,
Extrude cut the circle.
One relation: circle center and midpoints of both lines as horizontal (or vertical).
Dimension the remainder.
Extrude cut and circ pattern.
Kevin
Hi,
you can also save the sketch to the library with drag and drop. As well as a library feature or a block. It's also possible to save the complete feature to the library.
In your next sketch please use your center lines NOT like drawing them on paper. If you end the center lines exactly on the mid point of your contour (or vice versa), you'll define a symmetry of this line. And always think about using patterns. There a lot of possibilities in the sketch and even more with feature in your parts and assemblies!
Here's one way using a mirror and circular sketch pattern.. sorry just noticed I used arcs not lines for the outer entities.
...but here's a nice tip if you want to save a sketch to a library.
As others have mentioned SolidWork's wants you to save as a block, but as nearly always there exists a work-a-round.
Make a feature of the sketch.. ie an extrude.
Then drag the feature to the library (pin it open)
Once it's saved, close the file and open the library part. Just dbl click it
Now delete the feature then right click the sketch and select add to library
You will see this icon
Save the file and close it.
You can now drag in the sketch wherever you need it.
If you have external references you can add them (or just delete them from the libray part) see the help file.
You can even add configurations if you like.
If you want you can dissolve the library feature and end up back where you started
good luck
Ok Rob, I got it this far but your losing me on the process. I mean I think I can follow your instruction but
so are you saying I HAVE TO first extrude it before I save it ? Meaning I can't just save it as a sketch ?
Rob Edwards wrote:
Then drag the feature to the library (pin it open)
Once it's saved, close the file and open the library part. Just dbl click it
Now delete the feature then right click the sketch and select add to library
You will see this icon
Save the file and close it.
You can now drag in the sketch wherever you need it.
If you have external references you can add them (or just delete them from the libray part) see the help file.
You can even add configurations if you like.
If you want you can dissolve the library feature and end up back where you started
good luck
I'm pretty sure that's the way it used to work.
ie - You had to have a feature to create a library feature, but I just tried again and it worked!
You can select the file type here
F. Leatin wrote:
Ok Rob, I got it this far but your losing me on the process. I mean I think I can follow your instruction but
so are you saying I HAVE TO first extrude it before I save it ? Meaning I can't just save it as a sketch ?
Rob Edwards wrote:
Then drag the feature to the library (pin it open)
Once it's saved, close the file and open the library part. Just dbl click it
Now delete the feature then right click the sketch and select add to library
You will see this icon
Save the file and close it.
You can now drag in the sketch wherever you need it.
If you have external references you can add them (or just delete them from the libray part) see the help file.
You can even add configurations if you like.
If you want you can dissolve the library feature and end up back where you started
good luck
Hello,
As I mentioned previously, selecting the circle's center point and the arc midpoints, a vertical relation can be added and the 0.30 dimension isn't required (and it doesn't need to be duplicated).
Also, by creating construction lines on 45° and 135° (perp relation between these two), the driving entities, at 12 of the clock, can be mirrored as a circ pattern without the need for the hokey sketch pattern command.
It looks busy with all of the symmetry relations, but all is driven by only changing the upper cut or the center circle:
Kevin
I hear what your suggesting. Sounds like a good solution. I'll study it and see if I can figure out how to execute that method.
Thanks for the help.
TRY DYNAMIC MIRROR SKETCHING ... better yet start with two circles and then draw a few lines and use the trim function.
best of luck in your sketching learning.
I hear what your suggesting also. Sounds like a good solution. I'll study it and see if I can figure out how to execute that method.
Thanks for the help.
Draw one, circular pattern the rest.