[Solved] I don't understand how to use Techdraw

Discussions about the development of the TechDraw workbench
freedman
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Re: [Solved] I don't understand how to use Techdraw

Postby freedman » Sat Mar 09, 2019 8:58 pm

wandererfan » Sat Mar 09, 2019 5:03 am
In a perfect world we wouldn't have drawings, we'd just share the 3D model. But the world isn't perfect.
I want to hand off drawings with good traceability, part numbers, and revision numbers. Revisions are tough, production has a pile of drawings they work from, the only control I have is to add what revision of drawing I want them to use, I put it in the order sheet and hope for the best. :)

chrisb, I presume everything I ask for would be an option even if my words say otherwise.

I will post a few more pics here of what some of the structure could look like but I have what I need, FreeCAD is so flexible that projects can be structured in many ways. Different forces apply to system design, there are smaller companies that don't need much structure and big companies that need a bunch because they have 1000+ parts with revision levels.

Thanks
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bejant
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Re: [Solved] I don't understand how to use Techdraw

Postby bejant » Sun Mar 10, 2019 2:59 am

@freedman, when the model is at whatever stage you like, I can't see why you wouldn't use Part WB > Make Simple Copy and use TechDraw to make one or more TechDraw sheets of that Simple Copy.
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NormandC
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Re: I don't understand how to use Techdraw

Postby NormandC » Sun Mar 10, 2019 5:10 am

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 :D

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 :mrgreen:

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.
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NormandC
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Re: [Solved] I don't understand how to use Techdraw

Postby NormandC » Sun Mar 10, 2019 5:17 am

triplus wrote:
Fri Mar 08, 2019 4:31 pm
When i am satisfy with a technical drawing i usually save it in a SVG and PDF format.
+1 for PDF for documentation purposes, at work I feel like I'm the only one who's disciplined about revisions, I encourage others to keep revisions, even PDF ones. It's very useful when a specific CAD drawing document revision was not saved. The whole idea is redundancy. :D (we also have automated online backups every night, plus additional less frequent backups of the whole network drive stashed away in a separate location)

chrisb wrote:
Sat Mar 09, 2019 7:19 pm
Make the file read only, lock it away, kill everyone changing it.
Now let's not go to such extremes :D
chrisb
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Re: [Solved] I don't understand how to use Techdraw

Postby chrisb » Sun Mar 10, 2019 6:44 am

I voluntarily withdraw the last option and hope that nobody was harmed since that post.
wandererfan
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Re: I don't understand how to use Techdraw

Postby wandererfan » Sun Mar 10, 2019 2:48 pm

NormandC wrote:
Sun Mar 10, 2019 5:10 am
So please pretty please, don't stop on TechDraw development just yet :mrgreen:
reste tranquille. il y a encore des choses a faire. ne t'inquiete pas.

Thanks for the detailed description of how drawings work elsewhere. Screenshots would be great.
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NormandC
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Re: [Solved] I don't understand how to use Techdraw

Postby NormandC » Sun Mar 10, 2019 8:52 pm

I found out that you can download a Windows 10 image from Microsoft's website for free and install and run it with minimal hindrance without even registering it/purchasing a license. It's a change from the XP days. So I downloaded it an hour ago, will try to set up a VM so I can install our commercial CAD program (have to look into the license stuff but working from home is an allowed provision). I think it'll be easier for me to produce screenshots at home than at work.

I swore I would never run Windows on my home PC again... :cry: :lol:
freedman
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Re: [Solved] I don't understand how to use Techdraw

Postby freedman » Sun Mar 10, 2019 10:16 pm

wandererfan
It would be possible to make a "frozen" drawing where a "read only copy" of the shape(s) is preserved at the time of drawing creation, and the drawing uses the read only copy instead of the current Source shape(s). Once the frozen drawing is created, the time consuming HLR and repaint processes would not be needed again, so response time would be improved.
Would this frozen drawing carry any workable data (i don't know the shape structure), for instance could it be compared (with a recompute)to the original active shape for a difference? I feel this could be very useful anyway, if the frozen drawing had a unique icon (for the tree) we would know that it's a read only copy of some version. Maybe we could identify it as "out of date"? I presume It could be named and use copy&paste? This could replace the "create simple copy" and be much faster.

Thanks for the write-up NormandC, good reading.

As a side note, the "create simple copy" icon sure needs a change. I found posts where is was discussed but never implemented.
wandererfan
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Re: [Solved] I don't understand how to use Techdraw

Postby wandererfan » Mon Mar 11, 2019 12:37 am

freedman wrote:
Sun Mar 10, 2019 10:16 pm
Would this frozen drawing carry any workable data (i don't know the shape structure), for instance could it be compared (with a recompute)to the original active shape for a difference?
You're way ahead of me! I've made an entry on my TODO list for this, but that's as far as I've gotten so far.

Saving either the simple copy or the original source geometry with the frozen drawing object/document/file should be possible.
triplus
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Re: I don't understand how to use Techdraw

Postby triplus » Mon Mar 11, 2019 1:17 am

freedman wrote:
Sat Mar 09, 2019 5:25 am
Somehow I missed this post:
Postby triplus » Fri Mar 08, 2019 6:41 pm
If you know you will be going back in the design history and will do things such as add and remove Sketcher geometry. And when doing that, if you don't want for existing drawings to change.

Use Part CreateSimpleCopy and base the drawing views on such feature instead.
This might be the answer. If a drawing can be based on this "model without history" then it doesn't recompute and never changes. I will test this and post back. Outstanding, Thanks triplus. :D
freedman wrote:
Sat Mar 09, 2019 6:19 am
I will do more testing but that looks like the answer. YES! YES! YES!

If you want to make a drawing that can't be corrupted then take your model object and "make a simple copy". You then base your drawings from the simple part. Now you have a rock solid drawing that is based on whatever version you used to make the simple part. The simple part can also be copy & pasted into a new document which you can use to make drawings. This file can be assigned a part number and is static and locked in time.

Perfect! thanks again triplus.
Good to hear that and you're welcome. Note that it still makes sense to create a SVG and PDF counterpart. As for example a new version of FreeCAD or OCCT will get used and topology could still change. ;)

Much less likely but still possible!

P.S. In Assembly 3 effort some possible solutions and improvement were already explored. Such as TopoNaming algorithm, that will try to do the correct thing, when the topology changes. In addition there is the possibility of:
The screen cast above shows another solution, that is, to freeze a sub-assembly. Once frozen, the sub-assembly's PartGroup object will make a copy of all geometry shapes of its parts. Any subsequent changes to the parts will not be reflected.
Once an assembly is done, it is a good habit to freeze it. Besides the benefits mentioned above, it also allows to be partially loaded when linked externally.
https://github.com/realthunder/FreeCAD_ ... e-Assembly

Therefore do get involved in such discussions, when FreeCAD 0.19 development cycle starts. Express your opinion, on what TechDraw needs, and it can be explored if some of that can be generalized and provided by Assembly 3 effort as a result.