OK. I'm attempting to follow the training materials supplied with Solid Edge for Frame. Lesson 10 starts the process for documenting how to create a frame profile.
After several frustrating hours and the less than informative lessons I am here to ask for your help.
I have been able to create and use my own profile but I am unable to get any of the snap points defined. Lesson 12, "Snap Point" is, well, not a lesson at all.
So you move to Lesson 13. OK. Still nothing. Then 14 and 15 and 16. Lesson 16 actually starts to have some materials to help you understand what the actual process is to create a Frame Profile. Bad news here is that the directions don't work. When you attempt to run the macro while the sketch profile is active and you are in the sketch environment the macro reports: "This utility is not supported. Please use 'Frame Origin' Command." You already did this in Step 12! OK. So my logic says maybe we can define more than one origin point then. Nope. So. I'm stuck in a loop between Step 12 and 16. If only the macro would work!
Anybody out there that has gotten this to work?
Program Files\Solid Edge ST10\Frames\Frame Component Utility
Solved! Go to Solution.
@RyanM I don't think the Frame Component Utility is needed anymore since the Frame Origin command is in the Sketch environment now. It is setting the Default attachment point. After it is placed on the path, you have the oppurtunity to then click the Edit Cross Section option and then the Define Handle Point. After that is selected, then the handlepoint selection options will activate and you can then use a variety of methods that generate additional handlepoints that can be used as the attchment point.
@KennyG Thank you! That solved the mystery. Now if we can get the documentation updated! ;-)
Now, do you know how to get the holes into the profiles? I did have to chuckle at the documentation that says to use the larges hole as your surface. Well, that would be tough to define. I do have a gage curves setup as construction geometry in the profile sketch and a defined variable of GAGE to control those locations. But I see that information isn't being pulled into the assembly part and you can't view it from the edit state. That kind of information is quite important to the design.
see attached ST10 file. Its the largest i-beam you can get! So if you test it use a large path of around 100" x 100"
Thats some chunky beamage there @RyanM , even after using a 100" [2540mm] square path.
Holes are normally handled via "Assembly Features", and make config's to identify and ultimately make drafts for those members.
Design Manager Streetscape Ltd
Solid Edge 2019 [MP3] Classic [x3 Seats - Cloud Enabled]
Windows 10 - Quadro P2000
@SeanCresswell Yes it is a whopper. I've never had to use one of that big before. I'm assuming that would be used in a vertical column and not as horizontal member. But when testing things out I go for worst case scenario to start with. In this case a whopping W44x335 that's 44" deep and 335 lbs a foot!
Documentation says to put hole definitions in the frame profile and then as you mentioned use assembly feature. But I'm noticing that I can't access the profile that has construction line as the gage hole pattern. This tool could use some work if you want to use it in structural steel environments.
I've already noticed that the coping function is not what you would want for designing i-beams. It's using line to line coping. Need the ability to define offsets from web and flange of mating beam and ensure that a nice round is in the corner of the cutout. Maybe chamfer the ends to get rid of the radius that is left. It should be using a KDES value as a minimum so as not to interfere with mating beam inside radius.
OK. So now that I've done this exercise. I'm thinking that using standard assembly type workflow is going to be more efficient for i-beam and column type design. Any rebuttals? I hope I'm missing something?
@RyanMI am in no way an expert at Frames so I believe that when you are asking about the Holes in a cross section I'm assuming you are talking about the fact that you can add a cylinder as a construction surface through the component cross section file to then use it as an indicator of the centerline where holes are permissible. You would then use the Assemblies "Hole" feature to place the holes using the construction surface from the component profile as a guide to determine the placement. These can be turned on/off by using the shorcut menu on the Frame node in Patfinder and using the options under the Hole Location flyout.