Questions about the TechDraw workbench

[luggw1]

OS: Linux Mint 19.1
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.1.
Build type: Release
Python version: 3.6.7
Qt version: 5.9.5
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)

I recently finished my design for a latch for a rolater walker and generated the beginnings of drawings in the TechDraw workbench. I'm quite impressed with the capabilities it offers in presenting an engineering component for drafting purposes. However, I assume because the workbench is still young, there are many tools I found lacking such as the ability to apply labels with leaders, general notes, the diameter symbol and the radius symbol (R) to name a few. Are these capabilities present and I just missed them? I did browse through the other workbenches and didn't see what I was looking for.

I figured this was not really a problem as I could export them to DXF files and open them up in QCAD Pro, which I use for all my 2D CAD needs and finish them up there. I soon discovered a couple of issues with that approach though. First, the drawing format doesn't transfer, presumably because it's an SVG file? This was not a significant issue as I have a seed file containing a drawing format for QCAD as well.

Second, the parts in the DXF files were all about 50 times too big. I always draw objects 1:1 and scale them when placing them in the drawing format, just as is done in FreeCAD's TechDraw workbench, but I found when I imported the DXF exported from FreeCAD, I found I had to scale it down approximately 50 times to get it to actual size. What would cause an incompatibility like that to occur?

For reference, I've attached the model and one of the completed QCAD dxf files.

Thanks for the info.
Bill Lugg

[freedman]

I export CAD direct from Part Design to 2D DXF. TechDraw will do many things you want to do but maybe not all of them as yet. I'm so comfortable in AutoCAD with all it's tools, placing limitations on drawings is very frustrating to me so I still need to export.

The conversion from inch to mm is 25.4; 2x that is pretty close to 50. You always need to measue after a DXF is generated and verify the scale, it's always a multiple of 25.4 or 0.039370. Import an export settings get me everytime so I normally just get the DXF file into CAD and then scale.

[meme2704]

Hi
Certe Techdraw lacks a lot of features compared to other CAD
you can add R or other letter in front of the definition of the format, where you can also change the number of decimals
you can add an annotation text and "recover" the leading arrow by deleting the format
you have automatic diameter and R signs using the dedicated tool, or you can change the format manually by writing% 0f so you do not have a decimal place
it's work in métric, I hope so that work in inch too

[jmaustpc]

TechDraw Balloons now in master (0.19 dev)
https://forum.freecadweb.org/viewtopic.php?f=9&t=35392

Since you are in the USA, perhaps you are trying to use US customary units? If so there was a bug where the "R" did not show up for a radius when US Customary Units....its fixed but in master, might (or might not) be back ported to a future 0.18.2 release if one is made at some time in the future.
https://forum.freecadweb.org/viewtopic. ... us#p302337

Units in FreeCAD are just a GUI display thing, your items are always in their real size no matter what units are displayed, internally FreeCAD always uses mm to describe this real size. So when exporting to DXF this can on occasions cause complications, DXF was once in the old versions FreeCAD supports, unit-less. Even if DXF did support units, it only did so in some applications and I have heard before that not all handled it in the same way etc. but regardless some people here using DXF and likely some DXF applications, expect to use the reverse logic such that the Units defined in the DXF file and the actually value together define the real size of the object. In that case you need to use a dxf reading application that supports units and does so in a consistent manner...

DXF has been around for decades, it has been constantly extended and updated over the decades. So many applications say they support DXF but which version of dxf and which features of DXF is another matter.

Why export to DXF? Some people want DXF for other reasons like using it as a input file to control a laser/water/oxy cutter etc.. But in your case you seem to only want it to dress up your TechDraw drawing, presumably to print or create a PDF file from it. If so just export as SVG and edit the drawing in Inkscape.


One other tip, if you want to change the number of decimal places in a TechDraw dimension by adjusting the "%2f" value, you have to "untick" a setting in your TechDraw settings "use Global Decimals".

[freedman]

The reason I export is the toponaming issue, drawings can be corrupted. I'm hoping this is fixed soon and a then we can all use Techdraw.

[wandererfan]

there are many tools I found lacking such as the ability to apply labels with leaders, general notes, the diameter symbol and the radius symbol (R) to name a few.

Leaders will be along shortly.
General notes can go into Annotations, or, I suppose, into a Spreadsheet view.
Diameter and Radius symbols are displayed on Dimensions. There was a problem with dimension prefixes for multi-part unit systems (ex ft-in), but that was fixed recently.

First, the drawing format doesn't transfer, presumably because it's an SVG file?

The Template (page background) is indeed not exported to Dxf. This was intentional as most Dxf tools are quite adept at page templates. And yes the template is in SVG and SVG to DXF is hard. If transferring the page background is essential for you, make a Feature Request.

but I found when I imported the DXF exported from FreeCAD, I found I had to scale it down approximately 50 times to get it to actual size. What would cause an incompatibility like that to occur?

FreeCAD thinks in mm - always. So the exported DXF file is in mm. The versions of DXF that FreeCAD can export do not support units for geometry. Most DXF software can scale input to the local scheme. If you search the forum, you can find lots of light reading on this topic.

I would have expected the scale to be out by 25x, not 50x, due to interpreting mm as inches. Not sure where the additional factor of 2 comes in.

[luggw1]

FreeCAD thinks in mm - always. So the exported DXF file is in mm. The versions of DXF that FreeCAD can export do not support units for geometry. Most DXF software can scale input to the local scheme. If you search the forum, you can find lots of light reading on this topic.

I would have expected the scale to be out by 25x, not 50x, due to interpreting mm as inches. Not sure where the additional factor of 2 comes in.

The discrepancy here is because the part being exported was scaled 2:1. Two of the parts were scaled 4:1 and were approximately 100 times too big. I forgot to factor that in when formulating my original post. In fact if I had taken time to do that, I probably would have figured this out for myself.

Thanks for all the other pointers too, I appreciate the help.
Bill Lugg