reox wrote: ↑
Fri Mar 08, 2019 7:08 pm
How is this handled in comercial CAD packages?
I don't know all parametric CAD packages, but I've tried a few, and have been using one in particular (Solid Edge) for work for the past 12 years.
What all of them have in common which FreeCAD doesn't is multiple file types. You don't have a single document containing everything, you have separate documents for: parts, assemblies and drawings. Solid Edge even has a dedicated file type for sheet metal parts. So typically in FreeCAD, you would have one file type dedicated solely to TechDraw drawings, for example *.FCTdw or *.FCDrw or whatever. This filetype would only contain TechDraw pages, that's it. This means that no 3D view window would be necessary (which I guess would not be practical/doable right now, because TechDraw currently extracts information from the 3D view, like view orientation).
This approach has great advantages: you can open only the drawing document, or the 3D model document (which would be a single part document or an assembly document). The 3D model document would not be bogged down by multiple drawing pages, and the drawing document would not be automatically recomputed upon opening. The TechDraw document could even link to multiple 3D model documents. Another advantage is, open a TechDraw document and the TechDraw workbench would load automatically.
I really hope that FreeCAD gets multiple file types at some point. In my opinion, it will be essential to deal with large assemblies and large multi-page drawings. I believe this could be implemented while keeping the single document *.FCStd approach which works fine for smaller projects.
The key thing is, upon opening a drawing document, its views are not automatically recomputed. If you just opened the drawing, then a pop up message will open to inform the user that the views are in need of update. In a Solid Edge drawing, view frames (borders) aren't visible by default; they only appear when your mouse pointer hovers over the frame, or if it is anywhere inside the view frame. But, if the view is in need of a recompute, then the view frame will be displayed in thin grey solid lines. Since the view frames never show up on their own, you have a clear and unmistakable visual warning that the drawing view is outdated. Now, don't ask me how the software can find out that a view is in need of update, which means that the 3D model document it's linked to was modified after the drawing was saved last; but it does, even if the 3D model document has not been opened
. realthunder in his FreeCAD LinkStage3/Assembly3 fork has implemented a mechanism to link to external files, maybe it would make this possible to implement in TechDraw.
So, you've opened a drawing and got the message that you need to update it. You update it manually by pressing an update button; then, once you've updated the drawing and changes have been applied to the views, two things happen:
- Numbered revision symbols are appended/attached to dimensions that have changed. The default revision symbol is an equilateral triangle. So you will get as many of these triangles with a digit in it (1, 2, 3...) as there are changed dimensions after the drawing's update.
- A dialog window pops up containing a list of the changes in the form of a table with the following columns:
- Revision number (the same as the digits in the triangles)
- Change description: reports the nature of the change, such as: changed dimensional value, detached (for dimensions and annotations when they lost their link to the view's geometry), it even reports if an annotation has moved on the page.
- Original (previous) dimension value
- New dimension value.
When you select a revision number in the dialog, the corresponding revision symbol gets highlighted in the page (useful to locate it among many changes). You can close the dialog and the revision symbols will stay on the page; or you can click on a "discard" button that will clear the revision symbols from the page, before closing the dialog. If you don't clear the revisions, then they will remain listed in the dialog the next time you update the page, so they seem to be saved in some buffer; I don't remember if they're saved across sessions, I'll have to check that out.
Dimensions that have been detached (because of topological changes to the original 3D model) are not deleted, they remain where they were originally before the update, but they turn bright yellow; you can reattach them to the views with the mouse pointer by dragging a dimension's extension line end points to the desired vertex on a view. This can be accomplished while the dialog remains open; once a dimension gets reattached, the revision symbol and entry for it in the dialog is cleared.
Also, sometimes the link to the original 3D model document is lost (for example, the file was renamed independently, or moved or deleted): in that case, the views will open and display their last known state, and the view frames will have a bright yellow colour. A pop up message will also alert to the lost link to the 3D model.
I think it would be useful to have such a revision dialog in TechDraw at some point, I do understand it would require quite a lot of work.
I hope this made sense, if it's not clear enough, I'll try to dedicate some time in the coming week to produce some screenshots. No promises though, I tend to forget or lack the time during work days...
freedman wrote: ↑
Sat Mar 09, 2019 5:05 pm
1)Add the "Create simple copy" to the TechDraw toolbar. I guess that's OK, it's a Part tool, not sure.
TechDraw is about creating drawings, nothing more nothing less, IMO a tool for model creation (even if it's for a simple copy) does not belong there.
wandererfan wrote: ↑
Sat Mar 09, 2019 2:03 pm
I've always considered TD to be an "addon" to the 3D model. In a perfect world we wouldn't have drawings, we'd just share the 3D model. But the world isn't perfect.
Don't sell TD short
A drawing module is not a mere "addon", it is still (and will continue to be) an essential part of a CAD program, on the same level as the part creation module and the assembly module. There is still something to be said of the good old multi-projection drawing, and for many manufacturing processes, while we have not been all replaced by robots yet and the Star Trek replicator has not materialized, working with drawings - be they printed on paper or displayed on a computer display or tablet - will remain in use for quite some time.
So please pretty please, don't stop on TechDraw development just yet
chrisb wrote: ↑
Sat Mar 09, 2019 7:19 pm
A File containing a drawing that does not reflect the model is confusing if not dangerous. You start with dimensions from the drawing, look up details n the model and nothing fits - no thank you.
+1 in my opinion, it defeats the whole purpose of a parametric CAD program.