Help with Tutorial Draft_ShapeString

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DanaK
Posts: 28
Joined: Tue Nov 27, 2018 10:56 pm

Help with Tutorial Draft_ShapeString

Postby DanaK » Fri Nov 30, 2018 4:43 pm

The image shows the result of my attempt. I'm not removing the ShapeString from the block. Thanks for all your help

https://www.freecadweb.org/wiki/Draft_S ... g_tutorial

Result
Result of Turtorial Capture.PNG
Result of Turtorial Capture.PNG (20.87 KiB) Viewed 240 times
File
Engraving Tutorial.FCStd
(72.03 KiB) Downloaded 3 times
Last edited by DanaK on Fri Nov 30, 2018 5:11 pm, edited 1 time in total.
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HarryGeier
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Re: Tutorial Draft_ShapeString

Postby HarryGeier » Fri Nov 30, 2018 5:09 pm

Should be moved to Tutorials and videos
Kaum macht man´s richtig , gehts´s
My Video Tutorials on Youtube: https://www.youtube.com/channel/UCoe3B ... p8Q/videos
My FreeCAD Stuff on Hidrive: https://my.hidrive.com/share/qr3l1yddy6#$/
chrisb
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Re: Tutorial Draft_ShapeString

Postby chrisb » Fri Nov 30, 2018 5:11 pm

The problem is that the shapestring is coplanar with the surface. If you make the Extrude visible you see that there is nothing to cut. If you reverse it you are trapped by the frequently occuring coplanar issues with booleans. The following works:
- set the Reversed property of Extrude to true
- move Extrude a very tiny amount - e.g. 0.01mm - out. I used the transform tool available at double clicking Extrude and set the the increment to 0.01mm. Then I moved it with the blue arrow.
chrisb
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Re: Tutorial Draft_ShapeString

Postby chrisb » Fri Nov 30, 2018 5:12 pm

HarryGeier wrote:
Fri Nov 30, 2018 5:09 pm
Should be moved to Tutorials and videos
I was very unsure about the intention of this post and have now - after looking at the file - interpreted it as a help request.
DanaK
Posts: 28
Joined: Tue Nov 27, 2018 10:56 pm

Re: Help with Tutorial Draft_ShapeString

Postby DanaK » Fri Nov 30, 2018 5:56 pm

HarryG, I figure as much so added the help to title.

ChrisB, thanks that worked.

Would that mean the tutorial needs correcting. Perhaps. I looked it over to see if I had missed something. If so I cannot find it.

Thanks Again,
Dana
chrisb
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Re: Help with Tutorial Draft_ShapeString

Postby chrisb » Fri Nov 30, 2018 10:24 pm

DanaK wrote:
Fri Nov 30, 2018 5:56 pm
Would that mean the tutorial needs correcting. Perhaps. I looked it over to see if I had missed something. If so I cannot find it.
FreeCAD had always been picky with coplanar faces. This probably worked with some older version, but not with the current one of the underlying geometric kernel, OCC.

I will think about it, if there is a better solution than my quick shot, something like attaching the ShapeString to the chamfer.
chrisb
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Re: Help with Tutorial Draft_ShapeString

Postby chrisb » Fri Nov 30, 2018 11:17 pm

DanaK wrote:
Fri Nov 30, 2018 5:56 pm
Would that mean the tutorial needs correcting. Perhaps.
Dana, could you please try the following and tell me what you think about it:
- create the basic shape as before
- create the ShapeString as before

- switch to Part workbench
- Make sure the object "ShapeString" is selected in the tree view
- Use Part Extrude-Tool with the parameters:
-- Along normal
-- Reversed
-- Along: 1mm
-- Create solid

- Select ShapeString in TreeView
- Menu->Part->Attachment
- Select the chamfered face
- Select Plane face in the list; the ShapeString moves to the chamfer
- At the bottom of the attachment panel adjust x and y so that the ShapeString is positioned to your liking, e.g. x=2, y=-2
- Select Chamfer, then Extrude and make a boolean cut
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NormandC
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Re: Help with Tutorial Draft_ShapeString

Postby NormandC » Sat Dec 01, 2018 6:02 am

I've always found that tutorial needlessly convoluted. What people don't seem to realize (apparently Roland didn't) is that in Draft, if you select a face before creating Draft geometry, then the face will automatically be set as the working plane. So there is no need to make the ShapeString independently, create a sketch with a line then manually move the ShapeString to position. You may have to rotate it though, it could be oriented 90 degrees from what you wanted, but it will still be co-planar with the face.

Quick try: in this case, the ShapeString is oriented correctly. (EDIT: but I had made this cube in the same orientation as the tutorial)

phpBB [video]

(At 0:10 I'm showing that all snap modes are turned off)

There's one caveat to this method: the Draft working plane is a temporary thing, not like mapping a sketch to a face. So if you change the size of the cube, the ShapeString will stay where it is, you will have to change its position manually.

With the changes brought to PartDesign in v0.17, this can also be done in PartDesign, and I dare say more effectively. You can attach the ShapeString to a face on the Body, and create a Pocket. The advantage is that if you change the underlying solid, the ShapeString should update its position with it. The only thing is that the ShapeString will first be created outside of the Body, so you have to manually drop it into the active Body, then properly attach it to the chamfered face.

phpBB [video]


Normand
chrisb
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Re: Help with Tutorial Draft_ShapeString

Postby chrisb » Sat Dec 01, 2018 9:10 am

Personally I would always go the PartDesign way. Normand's video shows what to doand even more with giving insights in the dependencies. You can see (again) the advantage of PartDesign. The Part-way described in my post above is parametric as well, but it always needs the additional step of creating the extrude.

Dana, if you want to improve the wiki, you could update the wiki, perhaps with describing both ways.
DanaK
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Re: Help with Tutorial Draft_ShapeString

Postby DanaK » Sun Dec 02, 2018 4:44 pm

At this time I'm not feely all that confident to contribute. Spending time every day learning various methods to achieve a given result. Then doing it without instructions so to take notes one finer points. In time notes wont be needed and with a little luck understanding underlying concepts will result.