I only have three choices of tube in my drop menu, but there are many in the toolbox. Did something get missed in the install process?
I only have three choices of tube in my drop menu, but there are many in the toolbox. Did something get missed in the install process?
I have the choices in my ribbon toolbox but they do not appear in my library or weldment options. The weldment show the different types of structural style but then the choice of steel or aluminum then under steel graphics come up for the different styles but nothing after choosing the type. And the size square tube I am looking for is 2.5 sq x 11ga and its not in the toolbox.
If you're actually talking about Toolbox, as far as I know it doesn't work with weldments. It's been an odd thing from the start. You'd have to create the profile from the Toolbox definition then save it in the appropriate directory listed for weldments and be of the correct format, as Jeff has mentioned.
Do like Jeff says and download the profiles from the solidworks contenet folder.
Then make sure to place them in the folder shown in your system options. Ours are on the network so everyone is pulling from the same source and they can't be overwritten when a new installation of solidworks is done.
Once there they will need to be in 2 sub folders. The first sub folder is the pull down for standard (ANSI Inch) and the second is the folder for type (Tube). the third pull down is for the profile itself.
Hope this helps.
I know this is an older topic, but..just in case someone like me actually uses the search function before posting....
I tried 3 times to get the download to work properly. I was following the directions shown above - only I am a single user, so I was saving to the default location. No matter what I did, the downloaded file never showed up in the folder.
So, I downloaded it somewhere else...then unzipped it..then copied the contents and pasted them in the default folder.
This worked for me.
This is probably windows related, in the later versions of windows the Program Files directory is protected from being written to except with full admin access. It's probably not the best place for Solidworks to keep these files.
is it possible to pull the size and type of the weldment file into the cut list??
Jason Young wrote:
is it possible to pull the size and type of the weldment file into the cut list??
Yes, simply add those properties to your profile and they would show up in the cut list.
Deepak....
am all new to this??
can you explain this a little bit more?
or direct me to some more information?
You can open the profiles for editing in SOLIDWORKS just like any other SOLIDWORKS file. Now once you've it open, add the desired properties under File > Properties > Custom or Configuration tab (depending on how many configuration your profile has). And then when you use that profile for new weldment parts, the cut list would show those properties. For already exiting parts, you need to edit the feature, select a different profile and then re-select the same profile such that properties are updated.
I want to add to what Roy and Philip said about saving your weldment profiles.
1. When you open a new part and insert one of the profiles from Toolbox, edit the sketch so that the part origin will be where you want the pierce point to be when you use this for the Structural Shape function. When you use it you can change it, but it will default to the origin. Also add points anywhere you think you might want the pierce point to be in the future.
2. Exit the sketch, then click on it so it's highlighted, then save as .sldlfp.
3. If you're in a network environment, save them to your network so everyone can use them, as Philip said. If not, save them in "My Documents", or somewhere else on your hard drive. Not in the SolidWorks folder or they will likely get lost when you upgrade to a newer version of SW.
I use Weldments on just about every project, and it's a powerful tool, but it has to be set up correctly.
Here is what you are looking for. I made it from the TS2.5x2.5x0.1875.sldlfp file.
I just found another solution to the problem.
The Solidworks content standards downloads have the file path name in capital letters. The File path has to be in lower case.
No, nothing got missed. What you need to do is expand the 'SolidWorks Content' folder in your Design Library window. Click on the 'Weldments' folder. You'll then see a group of specs (Ansi Inch, AS, BSI, etc). Ctrl+click on the one you want to download a zip file of its profiles. You'll need write access to the folder C:\Program Files\SolidWorks Corp\SolidWorks\lang\english\weldment profiles so you can unzip said spec into it. You'll then have a slew of profiles to choose from.