I am not sure of the protocol here so please forgive me if I am stepping out of line or not following procedure.
I love Solid Edge, especially the flow from model to drawing. Taking an assembly of parts and preparing a set of drawings is smooth and effortless. I am not sure how many of you use the frame environment, there seems to be little on the forum group about it compared to other aspects of Solid Edge. I find this to be a fantastic tool. I am a freelance draftsman and design, develop and model for a wide range of customers. Having the availability to produce rapidly a frame is invaluable. But my customers do not need pretty 3D graphics to build the finished item they need details manufacturing drawings. That is at the very heart of solid edge, yes now we have additive manufacturing and Keyshot graphic for publications, but at the very heart is drafting. This is still what the engineer on the shop floor needs in his/her hands to make the item.
Frame is a fantastic tool to produce quickly a complex assembly of tubular components. It is now even more flexible with the use of synchronous parts are the foundation on which to build the frame. The flexibility and control in the frame environment has been well thought out and is very functional. Great job Siemens.
It is the very next stage in the workflow that I have raised the IR for and that is getting the frame assembly information to the drafting environment. This is the area where I would greatly appreciate your feedback and more over your support to get Siemens to seriously look at improving this aspect of the tool.
This image shows an assembly shows both part and sheetmetal components. Each component has it own unique document number, and title. Parts 1,2 & 3 are all exactly the same with the exception of the bottom leg. You could profile item 1 three times and simply saw off the bit not needed. Shown here simply to highlight the issue with the way frame operates at the moment. Items 4,6 & 8 are all the same part as well, differing in length and one having a feature added. Lastly items 7 & 9 are again the same part with one having a hole drilled in it.
Item 2 is a part copy of part 1, the same applies with part 3 being a part copy of part 1. I have repeated this for the SHS and the solid round parts. Being a part copy I get to give the copy a new document number and title.
In Frame this can also be achieved but only by one of two ways, both in my opinion are not a good solution. The first is to do a "Save As" on the frame. But this leaves a bundle of parts that have no association to the driving body or sketch. This takes away the flexibility of having the frame environment as well as increasing the steps needed to produce a finished product (ie. drawing).
The other method introduced in ST9 was the occurrence properties. This works in part with a few hacks. One is that you cannot have document numbers or titles for your original frame components (I will explain why shortly) and you have to change your table so that it shows both the Document Number and the Occurrence Number. See example below.
The image to the left shows the property box for adding the document number and Occurrence Number into the table. If the original frame component has a document number then the table will show both the document number and the occurrence number. This is the only way I could get frame, part, sheetmetal and assembly components to display their part numbers. I have done the same for 'Title'. You also have to manually work out which frame items are the same otherwise the table will show a list of document numbers on the one cell for each similar part you have given an occurrence number to.
If you want to show a single frame part on its own drawing sheet, then you need to hack the template to get it to work. I use the Document Number for the drawing number in my templates. However you can only use a graphic connection to get an occurrence number. This means the frame occurrence number cannot be in a template but on the drawing sheet. Then you need to lock the drawing view you have connected the call-out to otherwise the document number in the title will move.
What I would like to see is frame components coming into an assembly as a part copy just like the assembly in the image above. That these components also come into the assembly in a similar way in which holes in the synchronous environment are grouped. This grouping would be based on mass, length and or miter. That way all frame components in a groups would all have the same file name, title and document number.
This would then enable all frame components to be brought into the drafting environment the same way in which all other parts and assemblies do.
If you would like to see this sort of change in the frame environment then please make the effort to tell your VAR or what ever method is needed to tell Siemens that a change is needed. I would like to see the ease of use and flexibility of frame taken right through to the drafting environment.
Solved! Go to Solution.
Currently registered as IR 8867165. Not yet converted to an ER
Better append us to @Neil_H's "IR" also please.......This would make life easier dealing with frame based drawings, for sure. Currently we use many configurations to get the frame manufacturing info to the draft.
Design Manager Streetscape Ltd
Solid Edge ST10 [MP8] Classic [x3 seats]
Windows 10 - Quadro P2000
Testing: Solid Edge 2019
Thank you for the support Sean. Frame is an exceptionally good tool, it would be nice to have that same ease of functionality flow through to draft.
I like the frame tool for initial design, but have found that I am better off just modeling each stick because every tube needs tapped holes, cuts, etc and must be drafted on it's own.
If there was an easy way to export all frame members and assembly features to actual parts into a new assembly. Then the frame tools becomes useful as a starting place but would not be involved in the finished model.
The other thing that has lead to to making a model of each stick are downstream mates. For example. We make trailers. If I were to make a frame using the frame tool, but then needed to switch from 2x4 tubes to 2x6 tubes, and I switched out using the frame tools, all of the parts mated to the frame loose place. If I use an actual extruded part, then I can edit the part rather than switch out the frame member, and maintain all of the parts place.
One solution to this would be when you are initially choosing your frame member, you can make that part be inside of the folder you are working in. So you have your template tube member separate from your templates folder. Then, if what you are saying the dimensions of the tube needs to change, you can go into that part file and edit it. It won't have to go looking for a different file, and it will be the same faces according to the software. So you shouldn't lose any of those same relationships.
This is how I do it even when I don't use frame for shape steel structures. Because if a customer suddenly decides they want to change it from a W6x12 and up it to a W8x24, if I created all of my Parts of the structure with the very first feature being a part copy of W6x12 and have that inside of my working folder, and with the way I model from that point and with what I mate those members to, all I have to do is go into that original part file and change the dimensions in it, and then update the member parts, and I just saved my A$$ from the customers sudden change of heart and I can still hit my deadline.
@nominus38that is a good solution as long as the profile is the same. If the client says they don't want square hollow section but would prefer parallel faced channel then you have the same issue of re-attaching all the mates. Only if you are going to use the same profile and increase of decrease the size will that solution work. It becomes even more difficult if you the choice is made to change from rectangular hollow section to angle iron or pipe. Then you have a major issue to deal with.
To make the frame environment that flexible would be quite the programming miracle. Yet given that they are now bringing b-rep and mesh together then may be they will be able to re-establish broken mates?
This same issue applies however if your assembly is built up from an initial ordered part. Changing or deleting faces on that part will also create broken links in an assembly in the same way.