Symbols

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pgershon
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Symbols

Post by pgershon »

Hi folks,
I apologize if this is a dumb question. I am using v0.19. In the attached file, what do the 'tick' symbol adjacent to 'Sketch_Block2_CamHole' and the padlock next to 'Sketch_Block3_Bottom_ThruHoles' mean? I apologize, I don't know where to look up, like, 'Padlock symbol' and the symbol is too tiny for me to figure out what it is. Thanks.

Second question: If you open the 'Sketch_Block2_CamHole' and change the horizontal constraint from 10 to 8 mm, why does all hell break loose? :-) I mean it seems not to accept the new width when closing the sketch, and symbols then appear against other sketches.

Thanks a lot!

Paul
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Stage2k.FCStd
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edwilliams16
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Re: Symbols

Post by edwilliams16 »

https://wiki.freecadweb.org/Tree_view#Overlay_icons explains the symbols.

Your change to the dimensions altered the later geometry. It is a BAD idea to attach sketches to generated geometry - use offsets from the base planes if at all possible.
Screen Shot 2022-06-30 at 6.50.39 PM.png
Screen Shot 2022-06-30 at 6.50.39 PM.png (36.64 KiB) Viewed 603 times
You attached to a Face that got renumbered by the geometry change,

See https://wiki.freecadweb.org/Feature_edi ... ble_models
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thomas-neemann
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Re: Symbols

Post by thomas-neemann »

pgershon wrote: Fri Jul 01, 2022 4:27 am ...symbol adjacent to 'Sketch...
is that helpful?

https://wiki.freecadweb.org/Tree_view
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pgershon
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Re: Symbols

Post by pgershon »

Thomas,
Thanks, yes that was helpful, thanks: Diagnosis: "Object not attached to anything". Solution: Seems unsolvable on current Body, since I seem to have two sketches in conflict, I guess due to topological naming problem, and there is no way out using current drawing strategy of attaching sketches to generated geometry: In the attached file, I can delete "Hole", "Pocket006", "Sketch012", then create new sketch on "Rear" of Block3, to recreate the two concentric circles, but then the "Sketch_Block3_Bottom_ThruHoles" goes chain-link ("Not attached to anything").

I don't think I can successfully complete this task without a much deeper understanding of using FreeCAD along the lines of "Use offsets from the base planes" (edwilliams16). Right now I can't even figure out whether the current work can be rescued or whether I have painted myself into a corner and need to start again from scratch.

Best regards, Paul
thomas-neemann wrote: Fri Jul 01, 2022 9:03 am
pgershon wrote: Fri Jul 01, 2022 4:27 am ...symbol adjacent to 'Sketch...
is that helpful?

https://wiki.freecadweb.org/Tree_view
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Stage2L.FCStd
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pgershon
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Re: Symbols

Post by pgershon »

Ed,
Thanks that was helpful. I assume I need to master datum planes and try to generate a datum plane that coincides with the "Rear" of "Block3" of my part, and make pockets and holes in that plane, and this will resolve this conflict. So I started to study datum planes by creating one, finding it is "not attached", then pulling up a video that says "We are going to select our first reference, where we would like our datum to be. So I am going to select our XY origin", and the video got a reference to appear. I was unsuccessful clicking around everywhere I could think of in the 3D model, so I made sure it said "Selecting" then wen to the face I want the pocket to be in. Before going any further, am I going in the right direction? Should I try to change the size of the datum plane? Creatng shapes on this datum plane, is it still OK to constrain them to external geometry (edges of the original generated geometry)? I did this (attached file), but I am guessing I need to attach the sketch to the datum plane somehow, then somehow find a way to make pockets, which will need a bit more study or a hint (sorry about all this).

Best regards and thanks, Paul

edwilliams16 wrote: Fri Jul 01, 2022 4:54 am https://wiki.freecadweb.org/Tree_view#Overlay_icons explains the symbols.

Your change to the dimensions altered the later geometry. It is a BAD idea to attach sketches to generated geometry - use offsets from the base planes if at all possible.
Screen Shot 2022-06-30 at 6.50.39 PM.png
You attached to a Face that got renumbered by the geometry change,

See https://wiki.freecadweb.org/Feature_edi ... ble_models
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Stage2m.FCStd
(161.48 KiB) Downloaded 3 times
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thomas-neemann
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Re: Symbols

Post by thomas-neemann »

pgershon wrote: Sat Jul 02, 2022 4:04 am ...I guess due to topological naming problem,...
I would test it with the Realthunder version. there is the topo problem .... hardly available
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edwilliams16
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Re: Symbols

Post by edwilliams16 »

Here's a start, reusing your sketches. I used attachment offsets to place the sketches and expressions to make the offsets parametric.

See: https://wiki.freecadweb.org/Basic_Attachment_Tutorial
https://wiki.freecadweb.org/Expressions
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StageEW.FCStd
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Screen Shot 2022-07-01 at 7.54.26 PM.png
Screen Shot 2022-07-01 at 7.54.26 PM.png (83.6 KiB) Viewed 436 times
drmacro
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Re: Symbols

Post by drmacro »

Just a general comment about Datum planes.

Sketches have all the placement/attachment capabilities that a Datum plane has.

In a large percent of situations, using a Datum plane is simply redundant.

There are very good use cases for Datum planes, for arbitrary mirror or revolve axis for example.

But to support a single sketch, they are unnecessary and simply serve to clutter the tree view.
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Re: Symbols

Post by edwilliams16 »

You can cut down on the number of offsets required by a careful choice of the initial origin, so that the subsequent features align with the principal planes. I did this with your model. I didn't get around to renaming all the features, but you can walk through the model with the space-bar.
I used one Datum Plane, representing the bottom plane as it was the support for two subsequent sketches - Sketch005 and Sketch007. Other sketches were on principal planes or on offsets calculated by expressions, to make them parametric. External geometry in sketches only referred to previous sketches - the earliest available one in the tree, mostly Sketch.
You have two 6.35 mm dimensions, I made them independent. They could have been tied together, if that is the intent. This would have simplified some expressions.
This model, if you want to easily use it with different parameter sets, would be be well-served by coupling it to a spreadsheet. Then you wouln't have to poke through the model to figure out where any given dimension gets defined. I like using the DynamicData add-on in this situation.
This is all a little more work than just slapping sketches on generated geometry - but that leads to models that easily break under modification. For a one-off design, you might as well use Sketchup.
Screen Shot 2022-07-02 at 9.07.27 AM.png
Screen Shot 2022-07-02 at 9.07.27 AM.png (64.64 KiB) Viewed 346 times
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StageEW.FCStd
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pgershon
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Re: Symbols

Post by pgershon »

Folks,
I forgot to mention that I did go through the attachment tutorial. In the file "Stage2m.FCS2d" which I think is the file I attached above, there are two chainLink icon warnings for 'unattached' in that file. One of these is for "Sketch_Block3_Bottom_ThruHoles". I tried attaching this to the XY plane, and the chainlink disappeared, but this action flipped the counterbored holes upside down. I could not figure how to proceed from there. So then I tried attaching it to the top of the same block ("Sketch_Block3_Top_Slot") instead, but this did not make the 'unattached' chainlink go away.

I just cannot figure out how to proceed with this file.

I am very close to finishing this task, that is what is a bit frustrating (there was literally one final pocket remaining). I don't really want to learn a new program from scratch (SketchUp). I think it is better for my general education to persist with FreeCAD. The current piece may or may not be a "one off" job, it is hard to predict. However, it is for a one-off project, I am sure, since I am a non-engineer who may be over-reaching a bit.

I looked at Ed's very kind redraw of one of the three blocks, in file "StageEW.FSC2d". Just to confirm: This is supposed to be just one of the three blocks, not all three, I assume (I will check that I am not looking @ the wrong file after writing this post). I don't see the single datum plane mentioned in Ed's post. If I should use this as a basis for redrawing the whole piece, I will gladly give it a try, I guess there is no way to import or transfer sketches, so I will just generate new ones, which is fine, I can try this.

The 6.35 mm dimensions could probably be tied together if this helps, but I don't know how to do it yet.

Even I can now see ways I could have done this better: On block3 I guess I could have put both the slot and the screwholes in the bottom face instead of one in the top and the other in the bottom. Albeit both are generated geometry, it might have gotten me over the final hurdle perhaps.

Thanks for all the ideas in this post. I will follow up if I find I am misunderstanding something in the post.

Thank-you very, very much for your time and suggestions, Paul


edwilliams16 wrote: Sat Jul 02, 2022 7:17 pm You can cut down on the number of offsets required by a careful choice of the initial origin, so that the subsequent features align with the principal planes. I did this with your model. I didn't get around to renaming all the features, but you can walk through the model with the space-bar.
I used one Datum Plane, representing the bottom plane as it was the support for two subsequent sketches - Sketch005 and Sketch007. Other sketches were on principal planes or on offsets calculated by expressions, to make them parametric. External geometry in sketches only referred to previous sketches - the earliest available one in the tree, mostly Sketch.
You have two 6.35 mm dimensions, I made them independent. They could have been tied together, if that is the intent. This would have simplified some expressions.
This model, if you want to easily use it with different parameter sets, would be be well-served by coupling it to a spreadsheet. Then you wouln't have to poke through the model to figure out where any given dimension gets defined. I like using the DynamicData add-on in this situation.
This is all a little more work than just slapping sketches on generated geometry - but that leads to models that easily break under modification. For a one-off design, you might as well use Sketchup.

Screen Shot 2022-07-02 at 9.07.27 AM.png
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