I'm having a difficult time doing something I would consider very simple. Adding a rectagular hole to a frame component.
Lets say I have created a frame.
Then I use file menue save as...save selected model. Then picked the frame component and gave it a name.
I can then go edit that frame component and that file/part does contain the associativity paperclip. However when I go back to the assembly/frame, I still do not have a cutout in the frame.
I have updated all links, updated structure, and a few other things I can't remembers.
How do I make a frame that includes rectangular cutouts? I would like that hole to stay in place while the frame is edited. I also need to be able to draft the finished frame.
The obvius question at this point is how do I get the exported (saved as) part of the frame to actually live in the frame? The exported part is driven by the frame, but the frame in not using information from the edited part.
Solved! Go to Solution.
I have made some progress, but still dont have a complete solution.
I can create assembly features
export the frame part
Then insert that part into a draft file without the need to turn off 100 other frame parts.
What I was hoping for, is a way to isolate and edit a frame component that is still part of a frame. Allowing for editing of the frame that includes edits made to the indevidual part.
to restate the question: is there a way to create part driven assembly features and have that live linked to a frame assembly.
There is no simple way with one click now, but in the future...
I think you have to show assy feature on drawing view. I use some methods to show induvidual part on drawing.
Here is a video, what can be useful for you:
The way frames work is they take the cross section of the part and extrude it along the sketch lines you have selected. Other features will not be brought in.
There are two ways to do what you are doing. One is to make an assembly feature. Then you make a drawing viewof the whole frame and dimension the feature to the frame or you hide everything but the part in question in a drawing view.
The other way is to make a copy of the frame part with the correct dimensions and and insert it into the frame after deleting the instance of that part in the frame. I've done both. Sometimes in the same frame, but I don't reccommend it!
I came to the same conclusion. I was hoping there was something I missed and I could avoid using non-part driven assembly features.
This in turn deserves a feature request. When placing or editing view in drafting from an assembly, there should be a "SOLO" button for each part. Kinda like a sound mixer where you can only hear one track. In this case it would be used to only view one item out of an assembly....SOLO.
This is a need derived from what I call typical workflow. To me this includes detailing each indevidual part seperatly. Lets say I have a 50 part assembly. Then I need to detail 50 parts. I dont want to turn off 49 parts 50 times (2,500 clicks). I want to solo 50 parts.
You can turn off all the parts (uncheck "show") in the drawing view and then just turn on the one you want. Do this for one view and use that one to make the other views using "principal view" after you get it set the way you want.
I would start with the top part in the list and then copy the view when I had it all set (ctrl- drag) and then open display properties and check off the next item, then derive the other views from that again. I've never done this, let me know how it works.
Great solution to the part view management. Create a view with only one thing on (or 6, for the sides of a cube). copy that view, then just change what item is shown. Good time saver. I will be using this next week.