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

Discussions about the development of the TechDraw workbench
reox
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Re: I don't understand how to use Techdraw

Postby reox » Fri Mar 08, 2019 7:08 pm

How is this handled in comercial CAD packages? I never used them in production but got some training in Catia. If I remember correctly, the drawing would not update unless explicitly asked - but I could be wrong on that (it is some years ago already)

I think this is already implemented using the "Keep Updated" property of a page - right?
freedman
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Re: I don't understand how to use Techdraw

Postby freedman » Fri Mar 08, 2019 7:40 pm

I think this is already implemented using the "Keep Updated" property of a page - right?
It's more about the system than a flag like "Keep Updated". Imagine a production environment where you are in control of the model drawings, if someone needs a change and you modify the model there is a chance that all (lets say 10 drawings with 200 dimensions) will become corrupted. This could occur because of a big model change or topological errors. Can you imagine recreating all that, it could take days.
What I am proposing is that the model is not the most important piece of information in the file, the drawing is once created, it should never be able to be corrupted unless you are at file open and set a switch with probably a warning, maybe even a file check to test for "is there a backup of the file".
chrisb
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Re: I don't understand how to use Techdraw

Postby chrisb » Fri Mar 08, 2019 9:15 pm

I don't agree with this.If you want to keep a drawing, keep the model. What's the use of changing the model but not the drawing, if the drawing is so important. If something breaks it cannot be released as a new version until it is fixed, but not updating the drawing is not a solution for toponaming issues.
freedman
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Re: I don't understand how to use Techdraw

Postby freedman » Fri Mar 08, 2019 10:26 pm

What's the use of changing the model but not the drawing, if the drawing is so important.
In my case I moved one line over because something was a little to close (in a solid), I didn't want to change the drawing at all. But we have to update every drawing every time FreeCAD starts to see the drawings. I just wanted to look at my drawings, not change anything.
If something breaks it cannot be released as a new version until it is fixed, but not updating the drawing is not a solution for toponaming issues.
True. So we need some kind of plan for a toponaming error. Is it just to start over? Is it that we should have saved the drawing as a SVG and then go edit the SVG by hand? The topological issue and the model have been addressed, the same issue with drawings needs a proceedure to recover.
chrisb
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Re: I don't understand how to use Techdraw

Postby chrisb » Fri Mar 08, 2019 10:51 pm

I would guess that following the advice about how to create stable models will make the drawings stable as well. This is currently the only way I can see to avoid toponaming issues if you use the main 0.18 development version and not realthunders Assembly3 branch with improved toponaming handling.
freedman
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Re: I don't understand how to use Techdraw

Postby freedman » 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
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Re: I don't understand how to use Techdraw

Postby freedman » 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.

I'm sure wandererfan is reading this, is there some way this can be incorporated into Techdraw? Or what do you think about all this?
wandererfan
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Re: I don't understand how to use Techdraw

Postby wandererfan » Sat Mar 09, 2019 2:03 pm

freedman wrote:
Sat Mar 09, 2019 6:19 am
I'm sure wandererfan is reading this, is there some way this can be incorporated into Techdraw? Or what do you think about all this?
Honestly, I don't know the right answer. 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.

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.

Not obvious to me what happens when the frozen drawing is so out of step with the 3d model that it needs to be replaced. Delete the old one and make a new one?

If the drawings contain their own copy of the Source shape(s), then your idea of a separate document for drawings only becomes straight forward.

From a technical standpoint there is no obstacle to implementing this in v0.19. I'll have to defer to experts as to where such a feature would rank on the list of things to do.

Also don't know the relative merit of doing this procedurally vs marking a drawing "do not update" once you are happy with it vs doing this automatically.

wf
freedman
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Re: [Solved] I don't understand how to use Techdraw

Postby freedman » Sat Mar 09, 2019 5:05 pm

Here is the description for the Part tool "Create simple copy". (Dang, I can't figure out how to post the .png symbol...)
Removes the history of the part so that the different steps to create the part aren't accessible/editable any more.
With Simple copy only a non-parametric simple solid is produced, so if you want to change anything you have to go back to your creation file or history and fix the issue, then create a new simple solid.
Using the "Create simple copy" tool is perfect for creating a drawing, it is a container, the container can be named with part number, date, version. It also solves the problems with topological errors because the copy is never recomputed.

My thoughts are;

1)Add the "Create simple copy" to the TechDraw toolbar. I guess that's OK, it's a Part tool, not sure. I added it to Part design in a custom toolbar.
2) When inserting a view into a page, verify that the view is from a "simple copy". By definition, a drawing is a simple copy stored in time, the designer needs to add names, versions, dates..ect. for references, that's their job.

That's really about it. These steps can be done manually, but I think something like this will improve drawing/documentation. I'm doing just these steps already. Attached is a pic of what a model might look like with a production part that has gone thru some changes. Once the simple copies have been created they can be copied to a new FreeCAD file and then create drawings from that file. You could if you prefer, store your drawings in the current file but I like them separated out, then my model stays a model with very little overhead.
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chrisb
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Re: [Solved] I don't understand how to use Techdraw

Postby chrisb » Sat Mar 09, 2019 7:19 pm

wandererfan wrote:
Sat Mar 09, 2019 2:03 pm
From a technical standpoint there is no obstacle to implementing this in v0.19.
I am absolutely against such a feature. 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.

If you don't want the drawing to change leave the model alone. It's as simple as that. Make the file read only, lock it away, kill everyone changing it. But don't unlock the link between model and drawing.