how to construct symmetrical sketches

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scrungy_doolittle
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Re: how to construct symmetrical sketches

Postby scrungy_doolittle » Tue Jul 17, 2018 7:17 pm

scrungy_doolittle wrote:
Tue Jul 17, 2018 7:03 pm
You should consider to break it in several sketches. That would reveal the issues mentioned above and it would make each sketch simpler and easier to handle. You can use external geometry references to keep both sketches in sync.

The construction geometry should be deleted. The lines on the X and Y axis serve nothing but increase complexity. The construction lines at the 4 outer circles can be replaced with horizontal/vertical constraints on the points. The construction circle serves nothing but having the center in common with other points. Delete it and apply the coincidence directly.
The construction geometry is there to allow me to keep things in proper relationships when designing the next part. I do wish that there were layers to the construction, so you could work on sketches on layers, and have the underlying sketch be visible (the onion skin effect). The only way
I know to do that, is to create a sketch, then mark it as a construction line, so you can build on top of it. I'd love to learn some other way of doing it.

"outer circles can be replaced with horizontal/vertical constraints on the points"

How do I lock the center points of the 4 small circles to specific spots on the x and y coordinates?
What seems to be missing is a + constraint, that will lock a point to a line. the 0( constraint seems only to work with arcs and points.

horizontal and vertical constraints are measurement constraints as well.
When I opened Willhelms file, it complains about redundant constraints 25 and 32.
Is there a way to get it to ignore redundant constraints? In one case I was working on, it forced me to remove more than 20 constraints, and when I did and it was satisfied, geometry was skewed all over the place. That is a problem I have run into many times. Put in a constraint to lock something into relationship with something else, to prevent it from moving and that is good. Put another constraint, and it forces you to remove the first one.
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bejant
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Re: how to construct symmetrical sketches

Postby bejant » Tue Jul 17, 2018 9:09 pm

scrungy_doolittle wrote:
Tue Jul 17, 2018 7:03 pm
Here is the problem with doing that, I will have to unconstrain it, because the lines have to be moved, and the upper and lower arc chords have to be shortened without changing the radius, and then have to fully constrain it again.
With the Sketch open in Sketcher, why don't you simply double-click on the numeral 3.81 for the horizontal chords, or the numeral 4.38 for the vertical chords, and change the length?

Edit: more to follow.
Last edited by bejant on Tue Jul 17, 2018 9:59 pm, edited 1 time in total.
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bejant
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Re: how to construct symmetrical sketches

Postby bejant » Tue Jul 17, 2018 9:58 pm

scrungy_doolittle wrote:
Tue Jul 17, 2018 7:03 pm
Because of the following, how would you make separate sketches, and yet keep them in coordination where the internal features can be changed, while keeping them in specific alignments with the outer sketch, and not allowing the outer sketch to change?
Sketcher Carbon Copy (previously mentioned), or Expressions come to mind. The outer shape, once you have made it become Fully Constrained, won't change unless you change it.
Sketcher Cartbon Copy:
https://forum.freecadweb.org/viewtopic.php?f=10&t=21672
https://forum.freecadweb.org/viewtopic.php?f=9&t=21762

scrungy_doolittle wrote:
Tue Jul 17, 2018 7:03 pm
Secondly, freecad .18 has gotten into an odd state that makes it really difficult to do anything with.

wierdness.JPG
wierdness.JPG (389.56 KiB) Viewed 7 times

I can't seem to get it out of this way of displaying sketches, and it is almost impossible to see things when it is this way. Closing it down, restarting it and opening up the sketches, still leaves it looking like this.
You have chosen to display the Grid and, to make it worse, you have the grid spacing set to 1 um - that's 1 micrometer, or 1/1000 of a millimeter). Look at the left side of your screen grab and you'll see how to turn the grid off, if that's the "odd state" you mentioned. If something else is the problem, please clarify.

scrungy_doolittle wrote:
Tue Jul 17, 2018 7:03 pm
Trying to open Willhelms sketch to correct the outline (which is very wrong, but which I believe I can correct). At least it is fully constrained, so should be able to be constrained again.

Here is the problem with doing that, I will have to unconstrain it, because the lines have to be moved, and the upper and lower arc chords have to be shortened without changing the radius, and then have to fully constrain it again.

1. the top to bottom measurement i.e. the outer measurement from the outer edge of the arc to the corresponding arc need to be constrained to 14.5 mm

Open Willem's Sketch in Sketcher, double-click the 9.7mm Constraint, and change it to 10 mm.
10 mm between arc centers + r 2.25 mm arc + another r 2.25 mm arc = 14.5 mm top to bottom length.

scrungy_doolittle wrote:
Tue Jul 17, 2018 7:03 pm
2. the left to right dimension of the outer edge of the left and right arc needs to be constrained to 17.3
Double-click the 12.93 mm Constraint and change the value to 12.80 mm.


After this I think we're going in circles - this has all been discussed before. Why don't you first get the outside shape to your liking and we can go forward from there?
Bance
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Re: how to construct symmetrical sketches

Postby Bance » Tue Jul 17, 2018 11:37 pm

I think I have modeled basically what you are after, you can examine the included file by highlighting various bodies/features/sketches and using the space bar to toggle their visibility.

The master sketch 'outline' was created in sketcherWB and outside of a body, for speed I copy/pasted and drag/dropped this sketch into a body to create the basic pad, then added a pocket as needed for the various layers. BE WARNED this is NOT parametric and changes will not propagate. The correct way is to use a shapebinder as in body midplate0.7offset and use external geometry to the master sketch to accurately postion additional features.
symmetric.jpeg
symmetric.jpeg (47.4 KiB) Viewed 247 times
HTH Steve

OS: Linux Mint 18.2 Sonya
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.13983 (Git)
Build type: None
Branch: master
Hash: 8f1c6f77c090ae7d9c2bfd4f18811083b01a3eb2
Python version: 2.7.12
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 7.2.0
Locale: English/UnitedKingdom (en_GB)
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symmetrical_startBance.fcstd
(147.25 KiB) Downloaded 8 times
scrungy_doolittle
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Re: how to construct symmetrical sketches

Postby scrungy_doolittle » Wed Jul 18, 2018 12:09 am

bejant wrote:
Tue Jul 17, 2018 9:58 pm
You have chosen to display the Grid and, to make it worse, you have the grid spacing set to 1 um - that's 1 micrometer, or 1/1000 of a millimeter). Look at the left side of your screen grab and you'll see how to turn the grid off, if that's the "odd state" you mentioned. If something else is the problem, please clarify.
No, that was the problem. Thank you. I think that got turned on when I was chasing disconnected vertexes
bejant wrote:
Tue Jul 17, 2018 9:58 pm
Sketcher Carbon Copy (previously mentioned), or Expressions come to mind. The outer shape, once you have made it become Fully Constrained, won't change unless you change it.
Sketcher Cartbon Copy
I tried that earlier, but while it made a copy of the sketch, any changes made to one sketch affected the other, and that was *precisely* what I want to avoid.

So I waded through and got the various mid plates done, and have only to do the bottom plate. however, I would like to use part of a prior sketch in a separate file and copy it into my "master" file.
How does one accomplish this? Making the sketch visible, selecting the lines, there is no copy option.
selecting the sketch and then selecting the lines, likewise does not have a copy option.
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bejant
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Re: how to construct symmetrical sketches

Postby bejant » Wed Jul 18, 2018 2:31 am

scrungy_doolittle wrote:
Wed Jul 18, 2018 12:09 am
I would like to use part of a prior sketch in a separate file and copy it into my "master" file.
How does one accomplish this?
  • Open the file that contains the Sketch you want to copy, and also open the file into which you want to copy it.
  • Each file will be shown in a separate tab at the bottom of the 3D view window.
  • Click on the tab that contains the file into which you want to copy the Sketch (the "master" file), and this is the model you will see in the 3D view.
  • In the history tree, select the Sketch you want to copy, and do Ctrl + C, or from the pull-down menu choose Edit > Copy.
  • Press Ctrl + V, or from the pull-down menu choose Edit > Paste.
  • Now the entire Sketch is copied from the first file into the master file.
  • Change to the Sketcher WorkBench.
  • Scroll down to the bottom of the history tree and double-click the new Sketch that you just created in the master file to open it in Sketcher.
    Delete the geometry you don't want and close Sketcher.
  • In the history tree, click the Sketch you just edited to select it, press and hold down the Ctrl key, and click the Sketch with which you'd like to add the geometry from the Sketch you just edited.
  • Now you have two Sketches from the second file selected in the history tree.
  • In Sketcher, select the Merge Sketch tool:
    Image
    and this will combine the geometry from the two selected Sketches into a new Sketch.
I don't remember if the two original Sketches are kept or discarded, so you might want to make a copy of the second Sketch before using the merge Sketch tool.

Did you look at the file Bance posted? It looks like he did everything for you, although he used Part Design and I thought you were avoiding that WB.
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bejant
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Re: how to construct symmetrical sketches

Postby bejant » Wed Jul 18, 2018 3:06 am

scrungy_doolittle wrote:
Tue Jul 17, 2018 7:17 pm
The construction geometry is there to allow me to keep things in proper relationships when designing the next part.
Constraints would do that for you, but first you have to avoid the bad habit of failing to make your Sketches become Fully Constrained.

scrungy_doolittle wrote:
Tue Jul 17, 2018 7:17 pm
I do wish that there were layers to the construction, so you could work on sketches on layers, and have the underlying sketch be visible (the onion skin effect).
That's how the Part Design WB works, but previous Sketches have their visibility toggled to Off after they are used to create a Feature. Sketch, make a Pad of it, make Sketch001 on top of Pad, use the Pad tool on Sketch001 to create Pad001, make Sketch002 on Pad001, and so on. Or instead use Pocket on a Sketch to remove material from the model.

scrungy_doolittle wrote:
Tue Jul 17, 2018 7:17 pm
How do I lock the center points of the 4 small circles to specific spots on the x and y coordinates?
What seems to be missing is a + constraint, that will lock a point to a line.
Use the Fix Point Onto an Edge Constraint:
Image
to lock a point onto a line or arc, or onto extensions of lines or arcs.

scrungy_doolittle wrote:
Tue Jul 17, 2018 7:17 pm
Is there a way to get it to ignore redundant constraints?

No (and ignoring them is bad practice).

scrungy_doolittle wrote:
Tue Jul 17, 2018 7:17 pm
In one case I was working on, it forced me to remove more than 20 constraints, and when I did and it was satisfied, geometry was skewed all over the place. That is a problem I have run into many times. Put in a constraint to lock something into relationship with something else, to prevent it from moving and that is good. Put another constraint, and it forces you to remove the first one.
Pay attention to the Solver Messages. When you see a Redundant or Conflicting Constraint message appear, delete the Constraint you just added - it's probably the one that caused the problem.
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Re: how to construct symmetrical sketches

Postby scrungy_doolittle » Wed Jul 18, 2018 3:33 pm

bejant wrote:
Wed Jul 18, 2018 3:06 am
Constraints would do that for you, but first you have to avoid the bad habit of failing to make your Sketches become Fully Constrained.
Believe me, I try hard to make them fully constrained, but the degrees of freedom just seem to grow. For example, adding a construction line, adds 2 more degrees of freedom. Setting a length constraint on the construction line, may or may not reduce the degrees of freedom, depending on if it forces me to remove other "redundant" constraints.

I've even tried adding two items to a new sketch and constraining them. Generally can do that. add another and try to constrain it, generally causes more degrees of freedom.
So obviously I am doing many things wrong.
bejant wrote:
Wed Jul 18, 2018 3:06 am
No (and ignoring them is bad practice).
Not questioning that, but *why* is it bad practice?
bejant wrote:
Wed Jul 18, 2018 3:06 am
Pay attention to the Solver Messages. When you see a Redundant or Conflicting Constraint message appear, delete the Constraint you just added - it's probably the one that caused the problem.
I do that, but it just results in more degrees of freedom.

what is the difference between the |--| constraint and the <--> constraint?
bejant wrote:
Wed Jul 18, 2018 3:06 am
Open the file that contains the Sketch you want to copy, and also open the file into which you want to copy it.
Each file will be shown in a separate tab at the bottom of the 3D view window.
Click on the tab that contains the file into which you want to copy the Sketch (the "master" file), and this is the model you will see in the 3D view.
In the history tree, select the Sketch you want to copy, and do Ctrl + C, or from the pull-down menu choose Edit > Copy.
Press Ctrl + V, or from the pull-down menu choose Edit > Paste.
Now the entire Sketch is copied from the first file into the master file.
Change to the Sketcher WorkBench.
Scroll down to the bottom of the history tree and double-click the new Sketch that you just created in the master file to open it in Sketcher.
Delete the geometry you don't want and close Sketcher.
In the history tree, click the Sketch you just edited to select it, press and hold down the Ctrl key, and click the Sketch with which you'd like to add the geometry from the Sketch you just edited.
Now you have two Sketches from the second file selected in the history tree.
In Sketcher, select the Merge Sketch tool:
o.k. I have two files opened. one of that has a sketch 013 in it. one has sketch 001 in it and a broken extrude. Not sure at the moment why it is broken, but don't worry about that.

when I did a paste, the sketch came in on a plane XY plane, while the main sketch is on the z y plane. I have deleted what I don't want .

I found a re-orient sketch which did exactly what I needed.
So it looks like I am done with this particular journey.
Thanks to everyone who has contributed to it.

I probably still be asking questions.


I now have another question, but that needs to be it's own thread. I don't know how to split this thread. A related question, does anyone know how to download an entire thread and all files at once?

Lofting and extruding.
And that is:

how do I use lofting to re-create:
Final Part.pdf
(111.72 KiB) Downloaded 9 times
but without the obnoxious center line, and with and without the groove.

I believe that the best way is to use a non-grooved cross section, then create a "grooving" ring and do a boolean subtraction of the two.

This was done is solidworks, and that is the only source file I have for it. There was an earlier version that had an issue, and here is a pdf of the
construction loft schematic.
Loft Schematic2 in 3D.pdf
(49.46 KiB) Downloaded 8 times
This had the problem of a non uniform groove, and the ring cross section was not quite correct either. It was not drawn with a spline, so it did not quite have the correct comfort band profile.

I do have a version of this in stl format that I believe I can use, but hey, while I am learning freecad.....
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Final-PART-Assem-Ring All Surfaces 19.31x2.IGS
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bejant
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Re: how to construct symmetrical sketches

Postby bejant » Wed Jul 18, 2018 4:40 pm

scrungy_doolittle wrote:
Wed Jul 18, 2018 3:33 pm
For example, adding a construction line, adds 2 more degrees of freedom.
That's odd; adding a line segment (unless it is AutoConstrained onto some other geometry in the Sketch) should add 4 Degrees Of Freedom because, until the endpoints are Constrained, each endpoint is free to move in two directions.

scrungy_doolittle wrote:
Wed Jul 18, 2018 3:33 pm
Setting a length constraint on the construction line, may or may not reduce the degrees of freedom, depending on if it forces me to remove other "redundant" constraints.
If you have Redundant Constraints the Solver doesn't can't show the DOF until you fix the redundancy.
If you have Conflicting Constraints, the Solver can't calculate the DOF until you fix the conflict (the Solver can't know which of the Conflicting Constraints to use).
In either situation you should not add geometry into a Sketch until you fix the redundancy / conflict.

And until the Sketch becomes Fully Constrained there is ambiguity in it. You've seen a result of this ambiguity, when things change unexpectedly.

scrungy_doolittle wrote:
Wed Jul 18, 2018 3:33 pm
I've even tried adding two items to a new sketch and constraining them. Generally can do that. add another and try to constrain it, generally causes more degrees of freedom.
So obviously I am doing many things wrong.
Adding more geometry always causes more DOF, so that is to be expected, unless the new geometry is completely AutoConstrained as you create it (which probably doesn't happen often).

scrungy_doolittle wrote:
Wed Jul 18, 2018 3:33 pm
Not questioning that, but *why* is it bad practice?
Redundant Constraints mean that there is something wrong in a Sketch, and they cause problems for the Solver. You'll also see that once Redundant Constraints are detected, remaining DOF isn't displayed - the more important task is for the user to fix the redundancy.

scrungy_doolittle wrote:
Wed Jul 18, 2018 3:33 pm
I do that, but it just results in more degrees of freedom.
The next time this happens give us a how-to on recreating the problem, and upload the file so we can have a look at what is happening.

scrungy_doolittle wrote:
Wed Jul 18, 2018 3:33 pm
what is the difference between the |--| constraint and the <--> constraint?
The |--| constraint is the Horizontal Distance Constraint, and the other is the General / Overall Distance Constraint. Horizontal (and Vertical) Distance Constraints are preferred over the General Distance Constraint because they are easier for the Solver.

scrungy_doolittle wrote:
Wed Jul 18, 2018 3:33 pm
how do I use lofting to re-create:
As for me, I will have to look into that later...
scrungy_doolittle
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Re: how to construct symmetrical sketches

Postby scrungy_doolittle » Fri Jul 20, 2018 10:59 pm

Questions:
I've tried all this again from scratch, 1 item at a time.

So I have some specific questions about how to constrain items.

I started with 4 points, one on each axis and positioned the correct distance apart.
Just trying to anchor them to the x y axis so they cannot move. I finally was able to use 4 locks to constrain them. The o( tool would lock them to the axis, but they can still slide back and forth on the axis, even if distance constraints are used.
So, I created 4 circles on those 4 dots, and applied an equality constraint to those circles. I can change the radius and they all change. That is all well and good. and marked them as construction lines. I still can't get them locked to the screen grid, nor to a specific spot on the x and y axis, because doing other things result in complaints about the lock constraints being redundant and forces me to remove them.

At any rate, my goal at that point is to create 4 arcs on top of the construction circles, but not connected to them.
I have done that.

Now:
How can I constrain the arcs, so that the left and right ones are equivalent, and the top and bottom ones are equivalent. And more importantly,
*how* can I set the arc, so I can take one end of the arc and move it along the arc to shorten it, and have the other end of the arc move the same amount and in opposite directions? i.e. so the angle is change symmetrically around the x axis, and have it happen on the matching equivalent arc?
In the attached file, the only arc and circle that is behaving is the top one.
The left and right arcs can move in the x direction and it is hard to get them centered around the y (vertical line.) HOW do I lock them? I tried using a lock constraint, but that causes complaints.
I want the outer edges of the left and right arcs to be 18mm apart, and have a constraint that does that. But locking them so they don't move left and right, I can't seem to do. The sketch is currently complaining about constraints 28 and 29. if I remove those I get 18 degrees of freedom.
The diagonal guide lines also show up as having degrees of freedom.
IF you tag something as a construction line, How do you lock it?
The next issue with this file, assuming all the others are fixed, shows up when you move the blue circles, only the top arc stays locked. It seems that the other 2 arcs got locked to the construction lines, rather than to the 18 mm and 14.8 mm constraints.
How do you control which element is locked to another when all of the constraints are on top of one another?

So
1. how do you constrain and lock the left and right arcs such that any change made to one arc, is reflected in the other arc?
2. how do you constrain the left arc, so that when you move one of the ends around the construction lines the other moves the same amount so that the arc stays symmetrical around the x axis?
3. how do you break the constraint of the arc to the underlying construction lines?
4. how do you lock the construction lines to the plane grid, so they stay locked in relation to it?
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