I am new to Solidworks and need some help. I am trying to join two corners together of 4x4 structural steel in an assembly. I want the corners to meet at a 45 degree angle. The structural steel pieces lie in planes that are not 90 degrees to each other. Can somebody provide advice or fix this for me? I need all the help I can get. I have attached my parts and assembly files as well as a screenshot.
Thanks for the help Glenn. I got to step 4. I made a sketch on the face of the tubing but have no idea what you mean by the "Convert Entities". I need more description at step 4.
Riley Kelly wrote:
Thanks for the help Glenn. I got to step 4. I made a sketch on the face of the tubing but have no idea what you mean by the "Convert Entities". I need more description at step 4.
It's a sketch tool that creates lines, arcs, etc co-linear with model edges or other sketch entities. I can't post a screenshot right now, but if you can't find it otherwise use the Search command at the top right corner of your monitor.
Thanks Glenn. I found it and created it! I just cannot get the surfaces to match. Do I have to cut extrude to match them at the corners?
By the way, next time please Pack and Go your Assembly into a zip file and post that instead of individual files. That will make it much easier for us to open them.
How did you get the corners to match? I attached a screenshot of what happens to mine.
I used an easy method. This method has been shown in the following video.
My new part is not according to your dimension. You can change it as you want.
I'm not sure, and the internet and my network are incredibly slow this morning, so I won't be able to check. The only thing I can think of is that the faces of the large Part aren't at the same angle. Is that possible?
Yes you are correct Glenn. The faces are supposed to be at different angles. I am modeling an existing structure and it was not assembled with a drawing on hand. The structure was essentially "cowboyed" together without a lot of similar measurements. Thanks for your help. I believe this is as best as I will be able to get this.
Riley Kelly wrote:
Yes you are correct Glenn. The faces are supposed to be at different angles. I am modeling an existing structure and it was not assembled with a drawing on hand. The structure was essentially "cowboyed" together without a lot of similar measurements. Thanks for your help. I believe this is as best as I will be able to get this.
Yup. If the sides of the box are at different angles you won't be able to get the ends of the tubing to match.
By the way, if you'll be doing this sort of thing more than on rare occasions I'd highly recommend looking into using weldments. It can save an incredible amount of time. If you decide to try it I'll be happy to help, and will send you a few .sldlfp files to help get you started.
Hello, and welcome to the forum. I'm going to get pretty involved here, but I'll try to take it a step at a time. I'd post my files, but I'm using SW2020, so you wouldn't be able to open them.
1. To start, open your Part files and delete all those add-ons at the bottom of the tree. Next edit your sketch that created the first Boss-Extrude so that the origin is at the center instead of one end.
2. Add mates in the Assembly to fully define it's location. I don't remember exactly what mates were there, but delete any other than between the faces of the hopper and tubing. First a coincident mate between the bottom edge of the tube and the bottom surface of the hopper shell, then a symmetric mate between the tubing's right plane and the outer faces of the hopper.
Now it should be fully defined, and the ( - ) should be gone from the Part name in the tree.
3. Now create a new Plane in the Assembly, choosing the inside and outside edges of the hopper to define the plane.
4. Click on the tubing Part in the Assembly and choose the "Edit Part" icon. That will allow you to edit the part in the assembly, and reference other entities or components. Start a new sketch on the face of the tube that you want to extend and use "Convert Entities" to create sketch lines coincident to all the edges, inside and outside, then close the sketch. (Ignore the yellow lines in the screenshot.)
5. Use this sketch for a new Extrude. Choose "Up to Surface" and choose the Plane you created in the Assembly, and you'll need to select one of the long edges of the Part for the direction so it doesn't extrude perpendicular to the face of the Part. If the "Merge result" box is checked, un-check it.
6. The next part shouldn't need screenshots to save me some time. You can exit out of "Edit Part" mode, and open the Part. Use the "Mirror" feature to re-create the new extrude on the other end. Be sure to de-select the default "Features to Mirror" and select "Bodies to Mirror" instead, and then use the "Combine" feature to merge these three bodies into one.
7. Repeat the steps above for the other Part.