TechDraw: going to be useful

[liutas4x4]

What I found on current WB, 0.19_pre 18024.

1. The way for a selection is still terrible. If I choose some dimension, let's say horizontal, I should (in real must) to be able select point, lines and so on after choosing a tool. Until I choose a next tool or escape it. For now I am forced to play like with smartphone touchscreen - select something, go to dimension tool, push it, choose position. It is not acceptable way to the real routine workflow, with a lot of dimensions. Too many unnecessary moving of a mouse.

2. About Tolerances. While there are a way to issue negative sign to lower value, there are not a way to place positive sign. Plus sign is omitted voluntary. So, 80 +0.5/-0.5 looks like 80 0.5/-0.5. Not good for many applications.

3. Trailing zeros. If dimension is 80, it must to be 80, not 80.000. Also, 15.5 is not 15.500, especially if it has tolerance, that runs it to 15.520 min and 15.541 max. So, trailing zeros must to be truncated. If you like them, let it be an option for someone. But there must to the way to truncate them.
With one exception: if one limit has some meaning digits after point, the next must to have the same number of digits, even if them are zeros. For example: +0.041/-0.000.

4. There must to be a way to type-in Name of Tolerance. Let's say 15H9 +0.033/-0.000. I not found how to do it. It can be drop-down list there.

5. If "Units" are turned on, then the name of units must to placed after all digits, after tolerances, not in between dimension and it's tolerance.

6. While idea of Section View is acceptable, it is not working: section is placed in wrong angle. Also, while changing a position of cutting line for a section, it is not updated on the screen until OK is pushed. No preview.

7. Hatching is not working on Section View. Area is grayed, without possibility to change it to Hatch.


8. While choosing a pattern for a Hatch, I see *.dll files in the list. Awesome.


9. The way for applying center lines is additional trouble: instead of snapping to object, I must to choose something at the dialog and I will see result only after pushing OK.

10. After some operation, Template branch got exclamation mark, with Python console message: "FreeCAD_Doc_19f08e02-86e5-4806-a5bb-1748059a368b_d1848e_4788/A4_LandscapeTD2.svg.c0afb684-8847-48e7-8d1b-72fbdddf3213' failed.", while I does nothing with it.


It is enough for today ))))

You work is strongly appreciated. But there are a long way to go.
To be continued.

Sincerely,
Eugenijus.

[DeepSOIC]

3. Trailing zeros. If dimension is 80, it must to be 80, not 80.000

It is very well hidden.
1. Go to TechDraw workbench
2. Edit->Preferences->Techdraw-> TechDraw Dimensions
3. Untick "use global decimals"
4. Enter %g into Default Format field. OK.
Now, new dimensions shouldn't have these trailing zeros anymore.

You can specify custom format string for each dimension if you want.

[Jee-Bee]

FC is not the only one that have difficulties with this...
also Solid Works have strugles with this...
12.00 to 12 goes well but 12.50 to 12.5 don't works...

[wandererfan]

But there are a long way to go.

Thank you for your detailed feedback, Eugenijus. There is indeed a long way to go. Some comments:

1. The way for a selection is still terrible.
>>> this comes up periodically. The traditional FC UI is/was object-action (as in "with these objects, perform this action". In a word processor this would be select your text, then press "Cut"). Some people prefer the action-object paradigm (press "Cut", then select the text).
>>> this is slowly changing, I guess, as more and more functions use a TaskView dialog instead of the "objects, actions, change properties) approach.

2. About Tolerances. While there are a way to issue negative sign to lower value, there are not a way to place positive sign. Plus sign is omitted voluntary. So, 80 +0.5/-0.5 looks like 80 0.5/-0.5. Not good for many applications.
>>> As I've said many times, I am not a draughtsman, so please educate me. The "over" tolerance should always have a '+'? Or there should be an option to include it? Should the option apply to a particular dimension or to the whole document?

3. Trailing zeros. If dimension is 80, it must to be 80, not 80.000. Also, 15.5 is not 15.500, especially if it has tolerance, that runs it to 15.520 min and 15.541 max. So, trailing zeros must to be truncated. If you like them, let it be an option for someone. But there must to the way to truncate them.
With one exception: if one limit has some meaning digits after point, the next must to have the same number of digits, even if them are zeros. For example: +0.041/-0.000.
>>> @DeepSOIC gave you the high points for decimal places in Dimensions and I've added a bit to the Wiki after reading this comment. The over/under tolerances do not currently use the/any formatSpec.

4. There must to be a way to type-in Name of Tolerance. Let's say 15H9 +0.033/-0.000. I not found how to do it. It can be drop-down list there.
>>> You could add an Annotation with the Name of Tolerance near the Dimension text, but that is a hack. You could use this work around with the Balloon tool - see https://www.forum.freecadweb.org/viewto ... 92#p298694
>>> Where do the entries for the "Name of Tolerance" come from? I'm assuming there is no standard list?
>>> I should mention here that the current over/under tolerance implementation is a stop-gap under a full solution is developed. There is/was some prerequisite work required, most of which has been implemented.

5. If "Units" are turned on, then the name of units must to placed after all digits, after tolerances, not in between dimension and it's tolerance.
>>> so something like VALUE upper/lower UNIT? or VALUE UNIT upper UNIT/lower UNIT?

6. While idea of Section View is acceptable, it is not working: section is placed in wrong angle. Also, while changing a position of cutting line for a section, it is not updated on the screen until OK is pushed. No preview.
>>> what does "wrong angle" mean?
>>> the "no live update" issue is on the list to be fixed.

7. Hatching is not working on Section View. Area is grayed, without possibility to change it to Hatch.
>>> Hatching the section face is certainly possible (not convenient, but possible.). See picture.
>>> Svg hatching and Geometric hatching are due to be absorbed into a more general "Face Decorator".
>>> Historical note. Section View was implemented long before any hatching was available. The only way to distinguish the cut surface was to apply a colour. This will eventually be changed to default to a traditional hatched cut surface.

RotatedAndHatchedSection.png (17.66 KiB) Viewed 1407 times

8. While choosing a pattern for a Hatch, I see *.dll files in the list. Awesome.
>>> is this in the PropertyEditor? if so, I don't know of a way to apply a filter to the selection dialog.

9. The way for applying center lines is additional trouble: instead of snapping to object, I must to choose something at the dialog and I will see result only after pushing OK.
>>> which centerline please? There are view H/V centerlines (to be deprecated), Face centerlines, 2 line centerlines and 2 point centerlines.
>>> "live preview" is a widespread issue within TD. It used to be generally available, but was removed in many cases to limit the number of recomputes required (as you probably know by now, some drawings are terribly slow to update).
This will (probably) be sorted out as part of v0.19 development.

10. After some operation, Template branch got exclamation mark, with Python console message: "FreeCAD_Doc_19f08e02-86e5-4806-a5bb-1748059a368b_d1848e_4788/A4_LandscapeTD2.svg.c0afb684-8847-48e7-8d1b-72fbdddf3213' failed.", while I does nothing with it.
>>> are you on Windows? If so, then there was probably more to that message. Something along the lines of "Attempt to rename FreeCAD_Doc_XXXXXXXXXXXXXXXXXXXXXXXXX to FreeCAD_Doc_YYYYYYYYYYYYYYYYYYYYY".
>>> there is an issue on Win involving renaming of temporary files. issue #4085

Once again, thank you for your help.
wf

[liutas4x4]

It is very well hidden.
1. Go to TechDraw workbench
2. Edit->Preferences->Techdraw-> TechDraw Dimensions
3. Untick "use global decimals"
4. Enter %g into Default Format field. OK.
Now, new dimensions shouldn't have these trailing zeros anymore.

You can specify custom format string for each dimension if you want.

Thanks, DeepSOIC.

It really works on dimensions. But how about tolerances?

Look:

80 with tolerance with trails.png (25.43 KiB) Viewed 1375 times

For upper dimension it must to be +0.5/-0.1, not +0.500/-0.000.
For lower should be +0.48/0.00 or +0.48/0 - both are possible.
For the left it is different situation. Good representation is +0.45/-0.10, while +0.45/-0.1 is acceptable, but not preferred.

That say, zeros should be truncated. But truncating with respect to other tolerance, to the same number of digits after point, in the pair is appreciated. The Absolute Zero can be represented as 0 without nothing, even without sign.

Hope it is clear ))

Sincerely,
Eugenijus.

[liutas4x4]

FC is not the only one that have difficulties with this...
also Solid Works have strugles with this...
12.00 to 12 goes well but 12.50 to 12.5 don't works...

Yes.On my SW 2016 it don't work yet. But on 2019 it must to be corrected.

Yours,
Eugenijus.

[liutas4x4]

To wandererfan:

It very nice to hear this response from you.

I will do my best to answer and explain everything, but tomorrow.
It was a little bit hard day.

Yours,
Eugenijus.

[liutas4x4]

1. >>> this comes up periodically. The traditional FC UI is/was object-action (as in "with these objects, perform this action". In a word processor this would be select your text, then press "Cut"). Some people prefer the action-object paradigm (press "Cut", then select the text).
>>> this is slowly changing, I guess, as more and more functions use a TaskView dialog instead of the "objects, actions, change properties) approach.

Just compare workflow on 0.17 DD and 0.19 TD:


On DD WB (not perfect, but enough): https://drive.google.com/file/d/167UOW6 ... sp=sharing

and

On TD WB: https://drive.google.com/file/d/1wZJi3x ... sp=sharing

2. >>> As I've said many times, I am not a draughtsman, so please educate me. The "over" tolerance should always have a '+'? Or there should be an option to include it? Should the option apply to a particular dimension or to the whole document?

It is very simple.

Look:

RepTol.png (40.24 KiB) Viewed 1226 times

The first row is sample. Second row -- kind of formal representation. Third - while + and - value is the same.
If one of limits is 0, it can by represented as 0, 0.0, 0.0000 - first two are more common.

3. .. The over/under tolerances do not currently use the/any formatSpec.
[/i]

But, will, yes? "One sunny day", © J. Cash

4. >>> Where do the entries for the "Name of Tolerance" come from? I'm assuming there is no standard list?
>>> I should mention here that the current over/under tolerance implementation is a stop-gap under a full solution is developed. There is/was some prerequisite work required, most of which has been implemented.[/i]

There are complete tables, containing all possible names of fits, both for Holes and Shafts:

http://www.mitcalc.com/doc/tolerances/h ... cestxt.htm

BTW all tolerances, based on fits, are explained there.

5. >>> so something like VALUE upper/lower UNIT? or VALUE UNIT upper UNIT/lower UNIT?

VALUE upper/lower UNIT

6. >>> what does "wrong angle" mean?

SecView.png (41.71 KiB) Viewed 1226 times

Section view should to be rotated in direction of A-A arrows, in this particular case 90 deg clockwise.

7. Hatching is not working on Section View. Area is grayed, without possibility to change it to Hatch.
>>> Hatching the section face is certainly possible (not convenient, but possible.). See picture.

How to do it? It is more convenient against importing into Inkscape?

8. While choosing a pattern for a Hatch, I see *.dll files in the list. Awesome.
>>> is this in the PropertyEditor? if so, I don't know of a way to apply a filter to the selection dialog.

It is because of "all files" @ dialog.

Hatch.png (108.57 KiB) Viewed 1226 times

9. >>> which centerline please? There are view H/V centerlines (to be deprecated), Face centerlines, 2 line centerlines and 2 point centerlines.
>>> "live preview" is a widespread issue within TD. It used to be generally available, but was removed in many cases to limit the number of recomputes required (as you probably know by now, some drawings are terribly slow to update).
This will (probably) be sorted out as part of v0.19 development.

So, it is serious. Huh. I see.

10. ... is an issue on Win involving renaming of temporary files. issue #4085

[/i]

OK.


---------------------------------

Hope it helps )))


Yours,
Eugenijus

[wandererfan]

Some progress....

6. While idea of Section View is acceptable, it is not working: section is placed in wrong angle. Also, while changing a position of cutting line for a section, it is not updated on the screen until OK is pushed. No preview.
>>> section alignment has been changed.
>>> the section dialog now performs live update

8. While choosing a pattern for a Hatch, I see *.dll files in the list. Awesome.
>>> this has been fixed

10. After some operation, Template branch got exclamation mark, with Python console message: "FreeCAD_Doc_19f08e02-86e5-4806-a5bb-1748059a368b_d1848e_4788/A4_LandscapeTD2.svg.c0afb684-8847-48e7-8d1b-72fbdddf3213' failed.", while I does nothing with it.
>>> this has been fixed

[liutas4x4]

Nice done.

Thank you!

Eugenijus.