Techdraw workbench too cluttered and missing hole centres

[DaveGray65]

Hi

I've not posted this on the Techdraw section of the forum because the summary of what that section is about indicates it's only for discussion of techdraw workbench development

Migrating from version 0.17 to version 0.19.4 I've encountered a number of issues. Several of them have been sorted out by scrutinising the FAQs and manual but can't find how to resolve the following issues:
First issue: Two changes between versions 0.17 and 0.19.4 cause a more cluttered Techdraw workbench. I find that clutter frequently obscures errors in the drawing. This is a particular problem with the part shown in the attachments, which is one of the most complex parts that I have drawn. The two changes are:
a) Two arrows on circle dimensions: The "Version 0.17 circle dimension arrows.jpg" attachment is a scan of a paper drawing produced in version 0.17. As can be seen in that attachment, circle dimensions on Version 17 have only one arrow touching the circle. In the "Version 0.19.4 cluttered workbench.jpg" attachment, the circle dimensions have two arrows touching the circle, adding to the clutter. On the dimensions tab of the Techdraw preferences, the four Standard and Style options all have these two arrows. The techdraw preferences in version 0.17 did not offer Standard and Style options. The question that arises from this is, how can I select a style of circle dimensions that have only one arrow touching the circle?

b) Labels for annotations and views are visible: In the "Version 0.19.4 cluttered workbench.jpg" attachment, all annotations and views have visible labels, adding to the clutter. These labels are not visible in the version 0.17 techdraw workbench. As the labels are not visible in the printout, it shouldn't be too difficult to make not visible in the work bench. The question that arises from this is, how can I make the labels invisible in the workbench?

Second issue: No centre cross-hairs on some of the circles. In the "Bottom" view of "Version 0.19.4 cluttered workbench.jpg", several of the circles have no cross hairs. This makes it impossible to dimension the location of the centres of the circles. Some posts about this on the forum suggest changing the view's centre scale but I can't find anything about that in the manual. The question that arises from this is, How can I ensure that techdraw shows cross-hairs at the centre of all circles?

The part's Freecad file "Motor Cylinder head v1.12.FCStd" is also attached

Regards

Dave

OS: Windows 10 Version 2004
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.24267 +148 (Git)
Build type: Release
Branch: Branch_0.19.4
Hash: 476ecf091941bead59b14e44afa6064d5a66afa3
Python version: 3.8.6+
Qt version: 5.15.2
Coin version: 4.0.1
OCC version: 7.5.3
Locale: English/United Kingdom (en_GB)

[drmacro]

Have you looked at the plethora of updates and additions to TechDraw in 0.20?

[Shalmeneser]

a) Two arrows on circle dimensions
b) Labels for annotations and views are visible
c) No centre cross-hairs on some of the circles

a) You should be able able to erase them in Inkscape (svg export)
a) Diameter = 2 arrows / Radius = 1 arrow (you could use radius arrow with custom text of diameter)

b) TechDraw_ToggleFrame

c) View00? : ComboView:View : Arc center marks = true (also in TechDraw global preferences)
c) v0.20 : TechDraw_ExtensionCircleCenterLines

This PDF is about Production sequence : you should create one drawing per action (like IKEA sheet)

[papyblaise]

I'm only using V20 now, hope my answers will be updated
to remove text marks and outlines click on the "red circle and diagonal bar" button (prohibited)
to modify the slides in R you have to modify each dimension one by one, I did not find any change in "Preference" and you see that the symbol changes
I also changed the position of 6.83 so that it came out of the between-two lines

Edit : the diameters have become R, it would be necessary to force the value in diameter by hand, which forces them all to be taken over and unfortunately I do not know how to force the Diameter symbol, except to write a D

[0mer0]

a) Two arrows on circle dimensions

As a general rule, diameter dimensions are usually represented with two arrows and radius/arc dimensions with one arrow.
Anyway, in the case of diameter dimension representation, FreeCAD offers the possibility of changing the Rendering Extent property to the Reduced value to obtain the dimension with a single arrow.
(Personally I would not approve a dimension made in that way)

Edit:
Try to avoid dimensioning the hidden lines, for this, cuts or sections will be used.

Rendering_extent.png (83.05 KiB) Viewed 1367 times

[papyblaise]

Should have known, it is not on any tutorials

Edit
https://forum.freecadweb.org/viewtopic.php?f=21&t=69064
Indeed it is documented, but is misleading because it concerns all dimensions, it would be necessary to delete "Length"

[DaveGray65]

Many thanks for these replies which sorted out all of the problems I was asking about.

One question arises. In addition to making the annotation and view lables not visible, Techdraw|Turn view frames on/off also removes the outlines that enable things to dragged around the drawing. Is there a way of making the the lables not visible and still be able to drag things around the drawing?

[papyblaise]

by activating / deactivating once, we have access to annotations and movements just by clicking on the text and holding the mouse button

[DaveGray65]

Playing around found that right click offers “Toggle Frames”, which is much more convenient. Also found that, with frames not visible, it’s only the views that can’t be moved so that, by roughly positioning the views first, most of the work to be done without the cluttering labels. Then the final fine positioning of the views can be assessed, frames toggled on, views moved, frames toggled off and final positioning of the annotations and dimensions. That sequence is OK.