How can I use a flat plate as part of a weldment? I would like to show an angle and plate welded together.
how familiar are you with weldments?
start a new part.
insert the weldment feature.
extrude the plate.
draw a sketch for the angle
create structural member from sketch.
Does this then fill out the cut list properly?
I personally like to create a profile of the flat stock and use it as a standard weldment.
That's what we are doing here. I have several thicknesses of plate - both in Inches and MM. It works out great because the custom properties get filled in automatically. If you want a copy of our profiles - I will be glad to post them. I made different thicknesses but kept the width the same for all (300mm detault). So if you want a wider plate - just edit the base sketch once you insert the profile. If you want your width driven by something else (like keep the width the same as the frame under it) make sure to change the width dimension to "driven" and use a mate to tie the width to another member - althought there is a but with 2010 and it does not work well - give it a shot - you'll see what happens - SW - are you listenting.....
Hope this helps.
Hello John,
I am very interested in your profile library. If you could only send me a couple of profiles it would be great. Even better if you have a part file that shows the way you use the library.
We are making some prety complex welded structures using plates and I am trying to find the best tool for that.
Regards,
Marco
John,
I myself work with weldment cutlist and I have yet to figure out how to add a custom profile for different sizes of welment plates.
Hector, If you are using SW2013, you can create your plates using the Sheet Metal tools, and the cut list will populate automatically with the correct dimensions.
Patrick,
By using Sheet metal tools, you mean convert to sheet metal and set at my desired thickness? If this is what is meant by using the sheet metal tools then it did not work on my end, can it be my settings? We do have a custom welment cutlist, would that effect it in anyway?
Hector,
Welcome to the forum. If you want to have strap profiles available for the Structural Shape function, it's a fairly simple process, but it needs to be done right. Open a new part, create a sketch of the profile, exit the sketch, click on the sketch in the tree to highlight it, then save it as a .sldlfp file in the location specified at Tools > Options > System Options > File Locations. Frequent areas that cause problems are failing to exit the sketch, failing to have the sketch highlighted when saving as .sldlfp file, and failing to have the proper folder structure when saving the file (you need to have the right number of sub-folders, see here: https://forum.solidworks.com/message/360174#360174).
I am enclosing one of my files for you to look at if you want. You can also open it, edit it for different sizes, and save it as a different name if you wish. There is no need to have the sketch highlighted when making edits and saving, only when saving a .sldprt as .sldlfp the first time. It's also set up with a custom property, TYPE, which will carry over as a cut list property when used in a part. The property is linked to the dimensions so that if they are edited then property will update.
Also, since you're a new member, here is a discussion that has a lot of good information in it about the forum if you'd like to take a look: https://forum.solidworks.com/thread/39793. And feel free to ask if you have more questions.
Glenn
Glenn,
Thank you so much for your help, now I have another concern/dilemma. I have a custom cutlist where it shows me the description, length, width, mapics. With the profile you provided for the flat plate the cutlist does not automatically generate the information. What must I do to my settings or options in order to get the cutlist to read out this information.
Thanks,
Hector
You will need to open the .sldlfp file and add those custom properties, linking them to dimensions in the sketch, though length should be generated automatically without a seperate custom property. Then they should carry over to your cut list after it's updated. Keep in mind that this will only affect future use of the .sldlfp file, since when the Structural Shape feature is used it pulls the information from the .sldlfp file but it doesn't maintain a link to the file, so later changes to the .sldlfp file will not affect earlier uses of it.
Yes this was a great help.
Regards
how familiar are you with weldments?
start a new part.
insert the weldment feature.
extrude the plate.
draw a sketch for the angle
create structural member from sketch.