Bug 4687 Extension Line Direction in Iso Views - Help Please

Discussions about the development of the TechDraw workbench
Forum rules
Be nice to others! Respect the FreeCAD code of conduct!
User avatar
wandererfan
Veteran
Posts: 6268
Joined: Tue Nov 06, 2012 5:42 pm
Contact:

Bug 4687 Extension Line Direction in Iso Views - Help Please

Post by wandererfan »

I need a bit of help with issue #4687 / https://forum.freecadweb.org/viewtopic.php?f=35&t=58282

First question: does the convention of aligning extension lines with the iso axes apply to all 4 of our supported dimension styles?

Second question: does this picture show the desired result?
isoDimTest.png
isoDimTest.png (25.55 KiB) Viewed 2437 times
User avatar
Shalmeneser
Veteran
Posts: 9475
Joined: Wed Dec 23, 2020 12:04 am
Location: Fr

Re: Bug 4687 Extension Line Direction in Iso Views - Help Please

Post by Shalmeneser »

2) ok for me

1) which 4? a + (b+c) + (d+e) + (f+g)
a TechDraw LengthDimension.svg Insert Length Dimension: adds a length dimension.
b TechDraw HorizontalDimension.svg Insert Horizontal Dimension: adds a horizontal length dimension.
c TechDraw VerticalDimension.svg Insert Vertical Dimension: adds a vertical length dimension.
d TechDraw RadiusDimension.svg Insert Radius Dimension: adds a radius dimension to a circle or circular arc.
e TechDraw DiameterDimension.svg Insert Diameter Dimension: adds a diameter dimension to a circle or a circular arc.
f TechDraw AngleDimension.svg Insert Angle Dimension: adds an angle dimension between two straight edges.
g TechDraw 3PtAngleDimension.svg Insert 3-Point Angle Dimension: adds an angle dimension using three vertices.
User avatar
wandererfan
Veteran
Posts: 6268
Joined: Tue Nov 06, 2012 5:42 pm
Contact:

Re: Bug 4687 Extension Line Direction in Iso Views - Help Please

Post by wandererfan »

Shalmeneser wrote: Wed Jan 19, 2022 10:38 pm 1) which 4? a + (b+c) + (d+e) + (f+g)
Actually, I meant ISO Oriented, ISO Referencing, ASME Inlined and ASME Referencing.

Is there something special about angle and arc dimensions in an isometric view? I can't quite picture it.
Syres
Veteran
Posts: 2893
Joined: Thu Aug 09, 2018 11:14 am

Re: Bug 4687 Extension Line Direction in Iso Views - Help Please

Post by Syres »

wandererfan wrote: Thu Jan 20, 2022 1:37 am Is there something special about angle and arc dimensions in an isometric view? I can't quite picture it.
Looks like a good example at the top of the page : https://forum.librecad.org/Isometric-dr ... 19832.html
aapo
Posts: 615
Joined: Mon Oct 29, 2018 6:41 pm

Re: Bug 4687 Extension Line Direction in Iso Views - Help Please

Post by aapo »

Hello,

Please also have a look at this post by user domad: https://forum.freecadweb.org/viewtopic. ... 70#p550643

There, domad demonstrates how it is already possible to do correct isometric drawings with version 0.20. His method involves using the new helper tools to create cosmetic lines for the dimension endlines, which is admittedly pretty clever, but painstaking. Note that his method works perfectly for a model that has slanted faces, which could be a problem for a fully automatic algorithm. IMO, most useful would be a tool that would let the user to choose an edge in the drawing that the dimension endlines then would be parallel to, and also another edge that the dimension line would be parallel to. When creating a dimension, these directions could default to the isometric directions, but it'd be great to be able to change them afterwards (otherwise slanted faces would not work correctly).
User avatar
wandererfan
Veteran
Posts: 6268
Joined: Tue Nov 06, 2012 5:42 pm
Contact:

Re: Bug 4687 Extension Line Direction in Iso Views - Help Please

Post by wandererfan »

Do horizontal dimensions make sense in an isometric view? The "real" horizontal axis is tilted 60* so a dimension along the view's X axis just looks wrong.
User avatar
wandererfan
Veteran
Posts: 6268
Joined: Tue Nov 06, 2012 5:42 pm
Contact:

Re: Bug 4687 Extension Line Direction in Iso Views - Help Please

Post by wandererfan »

aapo wrote: Thu Jan 20, 2022 1:02 pm Please also have a look at this post by user domad: https://forum.freecadweb.org/viewtopic. ... 70#p550643
My eyes are much too old for the gif in that post. :(

aapo wrote:IMO, most useful would be a tool that would let the user to choose an edge in the drawing that the dimension endlines then would be parallel to, and also another edge that the dimension line would be parallel to. When creating a dimension, these directions could default to the isometric directions, but it'd be great to be able to change them afterwards (otherwise slanted faces would not work correctly).
The more I look into an automated solution, the better I like this idea.
aapo
Posts: 615
Joined: Mon Oct 29, 2018 6:41 pm

Re: Bug 4687 Extension Line Direction in Iso Views - Help Please

Post by aapo »

wandererfan wrote: Sat Jan 22, 2022 3:08 pm The more I look into an automated solution, the better I like this idea.
Yes, the well-known problem here is that after the 3D --> 2D projection TechDraw loses all the information about the 3D orientation of the faces. Unfortunately, the orientation of the faces (slanted faces) is required information for the isometric view dimension endlines. Thus, any isometric drawing of slanted faces in current TechDraw will most likely require user intervention for projection correction. Even more difficult case would be non-planar faces. However, I'm not sure how this worked in FreeCAD 0.18, maybe there was some kind of solution for these problems..?
User avatar
wandererfan
Veteran
Posts: 6268
Joined: Tue Nov 06, 2012 5:42 pm
Contact:

Re: Bug 4687 Extension Line Direction in Iso Views - Help Please

Post by wandererfan »

aapo wrote: Sat Jan 22, 2022 4:47 pm Thus, any isometric drawing of slanted faces in current TechDraw will most likely require user intervention for projection correction. Even more difficult case would be non-planar faces.
This is my proposed (manual) solution:
TaskDimension.png
TaskDimension.png (61.51 KiB) Viewed 2066 times
It appears to allow aligned dimension at any required dimension line/extension line angle. There are 3 new properties to control the layout of the lines, so a macro or future development could make what ever lines are required.
aapo wrote:However, I'm not sure how this worked in FreeCAD 0.18, maybe there was some kind of solution for these problems..?
The code in v0.18 was pretty simple as I recall. There was a table of isometric directions (eg (1, 1, 1)) and corresponding extension direction. The distance direction was compared to the table and the closest isometric direction (and extension direction) was substituted. it probably only worked correctly for certain directions.
aapo
Posts: 615
Joined: Mon Oct 29, 2018 6:41 pm

Re: Bug 4687 Extension Line Direction in Iso Views - Help Please

Post by aapo »

wandererfan wrote: Tue Jan 25, 2022 5:05 pm This is my proposed (manual) solution:
Wow! That looks good, and easy to use! Can't wait to see the drawings Domad will be able to do with this addition :D

I presume that the length information itself works like before, i.e. the user is supposed to link 3D-edges in the 3D-model to the desired 2D-dimensions/edges in the drawing. If I remember correctly, this works pretty well. Just link a Dimension to 3D geometry, and change the Dimension "Measure Type" Projected --> True.

However, the Dimension linking toolbox has a slight inconvenience in that it only let's the user select the edges from the 3D-view, and not in the 2D-view (i.e. the drawing). The 2D Dimension has to be selected from the list of all existing Dimensions, which is a bit cumbersome. Moreover, by selecting a Dimension in the drawing, and pressing the linking button, the linking dialog doesn't even open, but the program says "There are no 3D Edges or Vertices in your selection" even if the selected 2D Dimension already has already been linked to a 3D edge. My preferred functionality would be to activate the linking toolbox, press a "Select dimension" button, select a Dimension in the 2D drawing, go to the 3D view, press a "Select 3D edge" button, select a 3D edge, and finally press ok/accept for the linking toolbox. Sadly, this is not yet possible.
Post Reply