Part: Sweep: Path&Profile positioning

[sangue]

Can someone elaborate (maybe even in the manuals) how Part>Sweep treats the relation / coordinate systems between Path and Profile?
After two hours of tying, I still can't figure out how the positioning relation between the two has to be if they don't sit exactly at 0/0/0.

Simple example:
- A body with a Sketch as a path oriented in XZ
- A sketch with a line oriented in XY

Intention:
- Sweep the line/profile along the existing path, at the location of the path, to create a 'strip'.

Expectation:
- Traditionally, the profile is positioned normal to the start of the path
- Traditionally, distance and orientation of the profile points respect the vector point->path_start and path_start_normal.

FreeCad:
- It seems that the (world-)spacial relation between path and profile does only partially matter
- Apparently the distance is not measured in regard to the start of the path
- Trying to put the profile/line to different locations in world-space left the feeling that FreeCAD uses a 'shortest distance' (perpendicular?) from the profile to the losest point on the path.
- There is no possibility to move and 'snap' the endpoint of the profile-sketch to the start of the path-sketch in the part workbench (correct me if i'm wrong)
- The profile sketch can't be transformed and normal-oriented (at least not in an easy way).
- The profile sketch can only be lifted in direction of the sketch normal and shifted sideways with the position vector.
- The manual doesn't specify how that relation is interpreted
- Once the Sweep is made, there is no way to re-calculate the sweep (e.g. after nudging a point in path or profile)
- If the profile-sketch changes and that affects the world-spacial relationship between path and profile, redoing the sweep might lead to uncontrollable results.
- Even if the profile sits flush on the path, it might not follow the path.
etc...

See the screenshots below. the profile in white, the path in green.
The offset doesn't seem to follow an understandable logic, although I'm sure there is one and it would be nice to have that documented.

[TheMarkster]

To get a better chance of getting a good answer you should attach your file and provide the help -> about -> copy to clipboard information so we know exactly which version you are using.

Center the profile to the origin of the sketch, then attach it to the path. (Select profile sketch, in properties select Map Mode property, then click the [...] button to open that attachment editor.) The map path parameter (a value from 0.0 to 1.0) can be used to position the profile along the path once it is attached as a means of testing how the profile will proceed along the path.

[chrisb]

Center the profile to the origin of the sketch, then attach it to the path.

In another thread we just found that it can be essential to attach the profile to the path. At least the MacOS version doesn't work properly if this attachment is missing, even if they are aligned properly.

[sangue]

To get a better chance of getting a good answer you should attach your file and provide the help -> about -> copy to clipboard information so we know exactly which version you are using.

true! sorry! forgot! my bad....

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.4 (GitTag)
Build type: Release
Branch: releases/FreeCAD-0-18
Hash: 980bf9060e28555fecd9e3462f68ca74007b70f8
Python version: 3.6.6
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: German/Switzerland (de_CH)

[sangue]

Center the profile to the origin of the sketch, then attach it to the path.

In another thread we just found that it can be essential to attach the profile to the path. At least the MacOS version doesn't work properly if this attachment is missing, even if they are aligned properly.

it would be helpful to have the intended positioning concept/workflow in the docs (which is rather vague right now).
in my opinion it's difficult if the enduser has to guess the concept AND have platform-dependent inconsistencies in the way.
the clearer the docs, the easier it is for us to help with (potential) bug-reports.

[sangue]

Center the profile to the origin of the sketch, then attach it to the path. (Select profile sketch, in properties select Map Mode property, then click the [...] button to open that attachment editor.) The map path parameter (a value from 0.0 to 1.0) can be used to position the profile along the path once it is attached as a means of testing how the profile will proceed along the path.

wow... that recipe definately needs to go into the docs!!!
the docs don't even mention the whole attachment-part of the process (see Usage).

Thanks to TheMarkster, here's what worked for me:
1. Select the profile
2. Click on Map Mode > [...]
3. Click on Reference 1: > Select the first segment/line of the path from screen (SketchX:Edge1)
4. Set Attachment mode to "normal to edge" ('decativated' and 'intertia 2-3' both don't make sense - no other options available)
5. Set Yaw: 90deg to compensate rotation (optional)
6. Go to the Part WB > click Sweep
7. In the task dialog, activate the profile as 'selected profile' (right arrow)
8. Click 'sweep path' > go to tree view > select the path > go to task view > click DONE
9. click OK

comments:
- the sweep will be generated with placement 0/0/0.
- If the body of the path is not at 0/0/0, the placement of the sweep has to be corrected accordingly to match position.

[chrisb]

One additional step can be neccessary between steps 5 and 6: If the sketch is attached to the wrong end of the edge, change MapPathParameter from 0 to 1.

[sangue]

It should definately be added to the docs.

[chrisb]

It should definately be added to the docs.

I'm rather busy with other things. Why don't you register and add it yourself.

[Kunda1]

Where in the docs should this get added? issue #6079