If you like good old fashioned ballistics we you need to watch this video about using SolidWorks Simulation to create a Pumpkin Chuckin Catapult. This looks like alot of fun
Also for some great ideas check out this site.
For a good start in the your SolidWorks adventure check out his model from 3d Content Central.com
Have fun,
Bob McGaughey, CSWE
CATI
A common feature in the sheet metal industry are rolled edge flanges on a cylindrical parts. With all the great sheet metal tools that SolidWorks has to offer, that is one area the software has strugggled in the past. SolidWorks has never had the capabilitys to create a part as such and still be able to create a flat pattern from it. With the introduction of SolidWorks 2012, that has all changed. SolidWorks now has a new feature available in sheet metal that will allow you to create “Rolled Edge Flanges”. Its called “Swept Flange”. With this new feature, you now have the ability to create complex sheet metal parts and create flat patterns that go along with them.
Take a look at the example below...
Just like any sweep feature, you need to create both a profile and a path sketch (Note: with a sheet metal part, the path needs to be an open contour). Once you have your sketches, simply utilize this new swept flange feature located in the sheet metal features...
The results are just as you would expect...
However, as good as this new swept flange feature is, there is a slight problem when you go to show the flat pattern. You will get an error stating that this part cannot be unbent...
Fortunately, there is a workaround. The problem isn’t necessarily a problem with the geometry, but rather a problem with what SolidWorks thinks should be the fixed face/edge. If you edit the flat pattern feature, you can clearly see what face SolidWorks is trying to keep fixed...
To get this flat pattern to work correctly, you will need to select an edge to remain fixed; Just as you would if this was a rolled cylinder without the flanges...
Once you tell SolidWorks what edge is to be fixed, the flat pattern will work as expected...
SolidWorks does have a handful of SPRs out there that address this very issue on similar parts as you see here in this example. So if you run into a similar issue, look to see what SolidWorks is trying to keep fixed when flattening the part. Most likely, this workaround will resolve the issue.
Even with the workaround, the addition of this new “Swept Flange” feature greatly enhances the sheet metal capabilities in SolidWorks. You can now create more complex sheet metal parts than ever before.
Nathan Brunner, CSWP
Technical Analyst
Computer Aided Technology, Inc.
Working with a customer this morning I came up with a nice redneck workaround. This is what the customer as for.
Here is my Solution. Leverage a Feature Driven Pattern.
Start with a shaft with a hole in it.
Add Helix to part controlling the pitch. You can calculate the pitch by multipling the material thickness by 360, seeing that each part moves 1 degree instance.
Now use the Helix to create a Curve Driven Pattern.
Now insert that part in the assembly with one shim and perform a Feature Driven Pattern. The Feature Drive Pattern will update based on the patterning part. So you only have to change the curve driven pattern in the part to update the pattern in the assembly of the shim.
Also another hint so your pattern part does not show in your BOM. Right mouse button click on the pattern part and open component properties. Check the option for Exclude from BOM.
Enjoy,
Bob McGaughey, CSWE
CATI
The other day I got one of those questions. "I got a question, Bob. Can you take the points from a spline and save them out to a text file?" I was good up to the save them out to a text file. My brain threw the parking brake, "Ok say that again". You should always ask someone to repeat themselves when you think they are asking a stupid question. “So the real question was, “The user needs to get captured points along a curve or line into excel for a project.”
So we started to work on the issue. First off, there isn’t a save selected points to excel. This is going to need a work around. What formats can I save out of SolidWorks and can I read them in a tool like notepad or notepad++ easily. Take a look.
After saying out each one of these file formats, the one I thought of first was the best answer, IGES. IGES development began in late 1979 due to an increasing need to share data between CAD systems. While the IGES format is not the most powerful method for transferring CAD data, it is very common because it was one of the first detailed systems. This format was designed to be very open, and the data can be read in any text reader program. To learn more about the IGES format you can look at the Wiki page about it.
I didn't know IGES had a LOGO, cool!
http://en.wikipedia.org/wiki/IGES
Armed with this information I went add saved my part as IGES file. But the spline points didn’t show up in the IGES file the way I expected. In the IGES format the designation of 116 at the beginning of a line is a point. But I was looking for a line that had an X,Y,&Z values, but I was getting more than that. Going back to the model I created a new sketch and added points on top of the points of the spline on the original sketch. I resaved the IGES file and got much better results, which I copied to my clip board.
Now let’s get it into Excel. I pasted the data from the clip board onto a new text document. Excel can import a text file as a delimited file, where commas and colons with separate the data into cells. So there you go.
Cheers
Bob McGaughey, CSWE
Sometimes you may receive files from vendors or get information from a CCM where you need to plot out reference points using x, y and z coordinates. There are not many tools in SolidWorks that will allow you to enter in x, y, z coordinates regardless of the feature type.
One trick is using a 3D sketch…
In a 3D sketch:
1 - Create however many points you need. (Doesn't matter the location.)
2 - Select a point. Using the property manager on the left hand side, enter in the x, y, z coordinates of the point.
Note: Parameters for any entity in the property manager are strictly for reference. Entering values in the parameter boxes will NOT constrain the geometry. Relations and dimensions are highly recommended to fully constrain sketch entities.
3 - Because of the above note, the point is not constrained and is still floating in 3D space (hence the blue / under defined color). This is one of the few times that it would be a good idea to use the “fix” relation so that you do not in advertently move the point.
4 - Repeat the steps for the additional points.
Nathan Brunner, CSWP
Technical Analyst
Computer Aided Technology, Inc.
Surfacing Beginner,
You ever start a loft or a sweep and can't pick all the segments you need for a profile or guide. Well you should try the selection manager. It's found in the right mouse button click of the viewport when your in those type of commands. Here's example I did today.
As you can see it looks like the user was trying to loft 2 edges to a single edge. As you can see that didn't work. In comes the selection manager, which creates a selection group of multiple segments, edges, sketch geometry, that is treated as one element in the feature, awesome.... He cleared out the selection set and the right mouse button clicked in the viewport. Made his selections and hit the green check on the floating box to create that selection group. Stamp as DONE!!! as they used to say on Monster House.
Have great one, I'm off to do something... even if it's Wrong.
Bob McGaughey,CSWE
CATI
Rebuild Errors: "The end face cannot terminate the extruded feature"
In the extrude boss (adding material) and cut you have two a very powerful “end conditions” (what makes the extrusion stop) they are “up to surface” and “offset from surface”. Features go up to a selected face or SURFACE!!! and stop. The limitation is that you can only select one “face” on the model. So how can I make this happen you say? Well my friend it’s not a Redneck Workaround but we will call it one. YOU USE A SURFACE!!!
A surface by SolidWorks definition can be multiple faces knitted together. Let’s try to copy all those faces into a single knit surface. Where is the command? It’s actually the offset surface command. Change the offset amount to zero and the command is now the copy surface.
Now fire up the extrude command change to offset or up to surface, select your surface, and enjoy.
Bob McGaughey,CSWE
CATI Tech Staff
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