Lost my work and cannot find it

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jmaustpc
Posts: 10525
Joined: Tue Jul 26, 2011 6:28 am
Location: Australia

Re: Lost my work and cannot find it

Postby jmaustpc » Sun Nov 22, 2020 8:34 am

you have put all your sketches in different Bodies, a Body is just a single solid object, you should have used different sketches in the same body.

Also you still only have sketches you have not modelled a solid from the sketches yet. The sketcher is not intended for use as 2d CAD, it is top make profiles from which a solid can be modelled.

Your sketch with slots is not valid, because you have used a line in the middle of the slots to find their centres but you did not convert them into construction geometry.
Screenshot_20201122_192948.png
Screenshot_20201122_192948.png (10.2 KiB) Viewed 211 times
jmaustpc
Posts: 10525
Joined: Tue Jul 26, 2011 6:28 am
Location: Australia

Re: Lost my work and cannot find it

Postby jmaustpc » Sun Nov 22, 2020 8:38 am

select the line and convert to construction mode, by default they will be blue. And look like this...
Screenshot_20201122_193645.png
Screenshot_20201122_193645.png (9.24 KiB) Viewed 209 times
chrisb
Posts: 30704
Joined: Tue Mar 17, 2015 9:14 am

Re: Lost my work and cannot find it

Postby chrisb » Sun Nov 22, 2020 8:40 am

For how to center slots, you may look in the model I made: I used a geometric point which is symmetric between the centers of the arc. Then you don't need the additional measure of half of the side length.
You need at least FreeCAD 0.19.23300 to edit my current sketches.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
jmaustpc
Posts: 10525
Joined: Tue Jul 26, 2011 6:28 am
Location: Australia

Re: Lost my work and cannot find it

Postby jmaustpc » Sun Nov 22, 2020 9:09 am

Sketch039 was invalid because you had one extra random arc, I have deleted it.

Now your sketches will allow a Pad followed by a series of Pockets with "through all" and "reversed" selected.

Now you have a sold. Some of your sketches are not fully constrained but you do have a solid.

Now where to from here? I would suggest you just ask the laser printer if they can produce it from a solid object in a STEP file, if they can then just Export as STEP and send that to the laser printers.

Here is the repaired file... and a screen shot, note that even if you do only want a 2d CAD output li8ke dxf or similar, it is still worth modelling the solid as this shows that your sketches contained many errors that would have been less obvious in a 2d CAD format.
Screenshot_20201122_200620.png
Screenshot_20201122_200620.png (8.25 KiB) Viewed 190 times
chrisb
Posts: 30704
Joined: Tue Mar 17, 2015 9:14 am

Re: Lost my work and cannot find it

Postby chrisb » Sun Nov 22, 2020 10:10 am

Jim, if I add a 120mm constraint to your sketch "Holes" I would have expected it to be overconstrained, but it isn't. Do you get the same ok from the solver?
Attachments
Snip macro screenshot-44cc62.png
Snip macro screenshot-44cc62.png (18.44 KiB) Viewed 170 times
You need at least FreeCAD 0.19.23300 to edit my current sketches.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
jmaustpc
Posts: 10525
Joined: Tue Jul 26, 2011 6:28 am
Location: Australia

Re: Lost my work and cannot find it

Postby jmaustpc » Sun Nov 22, 2020 10:16 am

its likely that the laser cutters would prefer a DXF file since they at least used to use these commonly to define the cutting path.

If so just view from top view, select the solid and go File menu ...Export...select Autocad_dxf

If you want to view a DXF file easily its slightly less complicated if you just open it in a 2d CAD like LibreCAD.

Personally I would also export a simple TechDraw workbench drawing with just a few limited dimensions as a PDF file just to avoid any chance of confusion over scaling or units in the DXF file. So in other words, send both the pdf file and the dxf.

Here is an updated freecad file with a basic TechDraw drawing. and here is the dxf file exported from the above FreeCAD file.
serverbackplate.dxf
(45.31 KiB) Downloaded 3 times

OS: Ubuntu 18.04.5 LTS (KDE/plasma)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.
Build type: Release
Branch: unknown
Hash: 20649ec5292a31279f5593eccee2c5cd106bb099
Python version: 3.6.9
Qt version: 5.9.5
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/Australia (en_AU)
jmaustpc
Posts: 10525
Joined: Tue Jul 26, 2011 6:28 am
Location: Australia

Re: Lost my work and cannot find it

Postby jmaustpc » Sun Nov 22, 2020 10:34 am

chrisb wrote:
Sun Nov 22, 2020 10:10 am
Jim, if I add a 120mm constraint to your sketch "Holes" I would have expected it to be overconstrained, but it isn't. Do you get the same ok from the solver?
Hi Chris
Quite probably you are right, I just ran out of time trying to workout what was needed to fully constrain those not fully constrained sketches, there was a lack of consistency on how some things were sketched and it was quite confusing.

I had to cook dinner for my family and check on my goats etc. We had a few spots of rain so I had to run around moving the goat shelters into their current paddock so Chloe could take her babies out of the rain if it really came down hard, of course being Australia, as soon as I moved the shelters the rain stopped! :-) At this time of year or even in our winters its not nessecary to provide adult livestock shelter, its actually better for them to get rained on as it washes them a bit. But these new born kids are different, very small more delicate, for the first few days at least.

Honestly if I was doing this cover myself I would wonder if the triangles are worth the effort, if I wanted something similar I would probably just use round holes, but some fan vents are concentric curves like I did in my first attempt but more of them. Either way I would have considered modelling one set of vent holes and then using a Pattern feature for the other.

There may be a good reason for the slots but I suspect it is just to allow for sloppy size control and if so I would have considered just using round holes with adequate clearance to give enough wriggle room to get the screws to line up since the slots only give you flexibility in one direction and with modern cnc based manufacturing being so accurate and reliable it is likely that a round hole could be adequately precise. But I am guessing of course.
chrisb
Posts: 30704
Joined: Tue Mar 17, 2015 9:14 am

Re: Lost my work and cannot find it

Postby chrisb » Sun Nov 22, 2020 11:42 am

Based on Jim's file I want to make another proposal: I reworked the sketch and replaced some of the dimensional constraints, so that there are only 5 left instead of 14. I think that this way of constraining shows better the intrinsic symmetry. If the set of triangles should form a regular hexagon even more of symmetry could probably be used.

Then I added the bottom line of triangles. The overall number of constraints rose from 230 to 260, but that is a bit cheated, because I used quite some symmetry constraints consuming 2 DOF.

The pocket created by this sketch can then twice be mirrored to get the final result. This technique also reduces the filesize.
Attachments
X299-Case_cb.FCStd
(209.93 KiB) Downloaded 3 times
You need at least FreeCAD 0.19.23300 to edit my current sketches.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
chrisb
Posts: 30704
Joined: Tue Mar 17, 2015 9:14 am

Re: Lost my work and cannot find it

Postby chrisb » Sun Nov 22, 2020 1:52 pm

And here is another proposal, which I like even more, as it is made of only 4 triangles, and one multipattern. Furthermore it is more regular. However, if you prefer your shape of arranging the triangles you cannot use this technique.
The sketch itself looks like this:
SnipScreenshot-fe5901.png
SnipScreenshot-fe5901.png (41.25 KiB) Viewed 86 times
It is arranged around the origin of the sketch, and the AttachmentOffset of the sketch is used to position it on the base plate. The sketch has three dimensions which control 1) the size of the triangles, 2) the radius of the fillets and 3) the size of the gaps.
A polar pattern and a mirror then finish the task.

The file has again become a bit smaller, but what may be more important: with only 74 constraints the sketch can be handled (here) without any uncomfortable recompute delay.
Attachments
X299-Case_cb.FCStd
(177.5 KiB) Downloaded 7 times
You need at least FreeCAD 0.19.23300 to edit my current sketches.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
chrisb
Posts: 30704
Joined: Tue Mar 17, 2015 9:14 am

Re: Lost my work and cannot find it

Postby chrisb » Sun Nov 22, 2020 2:02 pm

Hi Jim, it took me quite some time to get this straight, so I missed your post from above until now. It is sufficient to know that you didn't add all constraints yourself, so I guess there is some issue with a previous step wich leads to the issue that the solver cannot recognize the redundancy.
Let's see what Abdullah has to say.
You need at least FreeCAD 0.19.23300 to edit my current sketches.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.