Step-by-step procedure for sizing the drawing
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.22319 (Git)
Build type: Release
Branch: master
Hash: 33ef4e0e35fba74c6e2fa3829cfd15c4b6f67e94
Python version: 3.6.8
Qt version: 5.12.1
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: Italian/Italy (it_IT)
1 - insert new standard drawing, by default it inserts the A4 sheet, to change it → structure → select Template → properties → Data → Template click on the button with 3 dots go to the installation root folder of FreeCad then click → Data → Mod → TechDraw → Templates and choose the one you want.
2 - model view → set the Front view
3 - structure → select object → click → insert view
4 - model view → set top view
5 - structure → select object → click → insert view
we select the views one at a time and set the scale to double
click on the view → properties panel → Data → record Scale = 2.0000
we insert the dimensions in the Front view
to insert the center line of the view we select the view → properties → view → record Vert Center Line = true;
left hole dimension
6 - select the two vertices (upper and lower) of the ellipsoid → enter the cosmetic line through two points;
(in the actions panel we leave everything as it is and click → Ok);
7 - reselect the two vertices of the ellipsoid → enter the two-point central cosmetic line;
in the actions panel we set the options:
- orientation → horizontal;
- extended by → 3 mm (or other value);
- style → at times (or other);
- click Ok;
8 - we select the cosmetic line of point 7 at the same time (ctrl key) at the vertex at the left base of the object → click enter Vertical dimension (6,50000 mm should appear)
- to limit the number of digits we select the quota and in the properties panel we modify the value of the “Format spec” record in% .0f (no decimal) or% .1f (one decimal) or other;
8.1 - we repeat the same steps for the other holes;
9 - select the vertices of the left side edge (object height) click → enter Vertical dimension.
P.N.
If any dimension is entered with an incorrect value, we can correct this value on the data properties panel → “Format spec” record, insert the exact value manually and in the “Arbitrary” record → set “true”;
we insert the dimensions in the top view
with regard to the standard dimensions of the diameters, I believe there are no problems, they are quite intuitive to insert;
10 - trace the center lines of the object, select the outer circumference and click on “Insert quadrant cosmetic vertex” → simultaneously select (ctrl button) 2 diametrical (vertical) cosmetic points → insert center line two points, in the actions tab click → horizontal orientation, extended = 4 mm, style = line-dot;
we do the same with the other two diametrical points (horizontal) by choosing vertical orientation and entering the other values equal to those entered before
11 - trace the center line of the hole on the left, select at the same time (ctrl key) the two points that define the diameter placed on the external circumference of the click object → two-point central cosmetic line, in the click actions → aligned , extended = 10 o 12 mm, style = dash-dot → Ok;
11.1 we use the same procedure for the other holes;
12 - we draw the lines of the left hole: since this hole has no references on the inner circumference, we insert two cosmetic vertices on it trying to put them parallel to the center line of the hole and aligned with those existing on the outer circumference, we select the inner circumference click → insert cosmetic vertex, in the actions tab click → Point Picker and define the insertion point on the circumference; we do the same for the insertion of the other cosmetic point;
13 - draw the dotted lines at the edge of the hole: select at the same time (ctrl key) the cosmetic vertex of the outer circumference and the aligned one (which we created) placed on the inner circumference → click insert cosmetic line two points and in the actions tab click Ok;
we do the same with the other two points;
14 - since the other two holes have the references on both circumferences, we trace the cosmetic lines in strokes that define the holes geometrically, the procedure is the same as in point 13;
now we are ready to indicate the angular dimensions of the direction of the holes
15 - we section the vertical centerline of the object and at the same time (ctrl key) the inclined one of the left hole click → enter angle dimension (it should appear 50,0000 °) in the properties tab → Data → record Format spec =% .2f now the value is 50.00 ° or % .0f for the value 50 °;
16 - we do the same to indicate the other angular dimensions of the other holes;
we indicate the size of the hole diameter with the conforming symbol (⌀)
17 - hole on the left, select at the same time (ctrl key) the vertices placed on the outer circumference → enter dimension length aligned, in the property sheet → Data → record Format spec = ⌀% .2f (copying the symbol ⌀ from the word wrinter and then pasted), now the dimension value is ⌀6.00 or with ⌀% .0f it becomes ⌀6;
18 - we do the same to indicate the other dimensions of the holes;
19 - we can now indicate the other dimensions that interest us the external and internal diameter of the object (⌀40 and ⌀30) with the appropriate function insert dimension diameter;
20 - if we want we can insert the 3D axonometric view and eventually define notations and other useful things for the construction of the object.
I hope my English translation is clear and understandable.
If any step is doubtful, you can ask for clarification
As you have experienced, the steps are many, slow and not very intuitive, (think how long it would take for a very complex drawing and how many cosmetic points should be inserted without considering the low precision) I therefore believe, turning to the developers, that the Draft tools should be extended in TechDraw but above all the snaps tools.
Happy Sunday to the whole community!
