Solidworks to FreeCAD Sketch questions

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michav
Posts: 2
Joined: Mon Sep 09, 2019 7:34 am

Solidworks to FreeCAD Sketch questions

Postby michav » Mon Sep 09, 2019 7:38 am

Hello Freecad forum,
Some questions regarding sketching

1. how to automatically mate a reference line to the midpoint of a sketch line

2. automatic constraints not working properly (its checked in my options but my lines are not automatically snapping to midpoints)

3. how to display sketch's and planes from one body, if im working on another body

4. if I am working on sketch B, how to snap to points in sketch A? is there a way to do this without the use of shapebinder?

Thanks!!
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HarryGeier
Posts: 1155
Joined: Mon Jul 10, 2017 12:36 pm
Location: Hof Germany

Re: Solidworks to FreeCAD Sketch questions

Postby HarryGeier » Mon Sep 09, 2019 9:41 am

michav wrote:
Mon Sep 09, 2019 7:38 am
Hello Freecad forum,
Some questions regarding sketching

1. how to automatically mate a reference line to the midpoint of a sketch line

2. automatic constraints not working properly (its checked in my options but my lines are not automatically snapping to midpoints)

3. how to display sketch's and planes from one body, if im working on another body

4. if I am working on sketch B, how to snap to points in sketch A? is there a way to do this without the use of shapebinder?

Thanks!!
#1 not yet possible, i think i was reading that this is a solver limitation
#2 same..
#3.You can see them , as long as they and the body are visible. Not for construction lines which are only visible in actual sketcher context
#4. When in the same body you use external geometry. Outside the body you use shapebinders or carbon copy.
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kisolre
Posts: 1360
Joined: Wed Nov 21, 2018 1:13 pm

Re: Solidworks to FreeCAD Sketch questions

Postby kisolre » Mon Sep 09, 2019 9:54 am

#1 easiest way add point, create symmetry of edge vertices around that point. This will put it in the middle.
chrisb
Posts: 19042
Joined: Tue Mar 17, 2015 9:14 am

Re: Solidworks to FreeCAD Sketch questions

Postby chrisb » Mon Sep 09, 2019 12:32 pm

I am not familiar with the Solidworks notions, so you may need to explain better what you have done.

You are talking about snapping and sketches. These two don't go together. Snapping is used in Draft workbench and sketches in, well, Sketcher workbench.

If we are talking about Sketcher:
#3: While editing the sketch you can switch to the Model tab and change the visibility in the tree view.
openBrain
Posts: 2183
Joined: Fri Nov 09, 2018 5:38 pm

Re: Solidworks to FreeCAD Sketch questions

Postby openBrain » Mon Sep 09, 2019 1:41 pm

michav wrote:
Mon Sep 09, 2019 7:38 am
1. how to automatically mate a reference line to the midpoint of a sketch line
No real automatic way. Midpoints are not supported. The best way is as explained by @kisolre to add an extra point and constrain it to be symmetric between the 2 line endpoints. You can do that by just selecting the line + the extra point and clicking on symmetry constrain.
In case it may help, I attach (very) basic macro that will add midpoint in this way to all selected lines on a sketch. You can bind the macro with an icon and a keyboard shortcut if you use it very often.
2. automatic constraints not working properly (its checked in my options but my lines are not automatically snapping to midpoints)
Auto-constraining works correctly in the extent of the supported constraints. :D
3. how to display sketch's and planes from one body, if im working on another body
Basically just make them visible in the tree view. ;)
4. if I am working on sketch B, how to snap to points in sketch A? is there a way to do this without the use of shapebinder?
The other way is to use Sketcher CarbonCopy (as Harry told). Each way has its pros & cons. :)
chrisb wrote:
Mon Sep 09, 2019 12:32 pm
I am not familiar with the Solidworks notions, so you may need to explain better what you have done.
In SolidWorks, when your mouse pointer is close to a line midpoint, a "handle" appears there and you can use it as a snapping point to eg. start or end a line.
You are talking about snapping and sketches. These two don't go together.
Don't totally agree with that. Mainly when using auto-constraining, there is some snapping effect (in the general meaning of the word). Say when you start a line, if you're close enough to an endpoint, it will add coincidence. Close enough to an edge it will add a point-on-line. Etc. ;)
Attachments
AddCenterPoint.FCMacro
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chrisb
Posts: 19042
Joined: Tue Mar 17, 2015 9:14 am

Re: Solidworks to FreeCAD Sketch questions

Postby chrisb » Mon Sep 09, 2019 1:48 pm

Ok, so we talk in fact about Sketcher here. Just to mention it: Snapping to midpoint exists in Draft WB.
openBrain wrote:
Mon Sep 09, 2019 1:41 pm
Auto-constraining works correctly in the extent of the supported constraints. :D
Sad to say, but using autoconstraints is to a certain extent a property of the sketch. If you have autoconstraints disabled when you first create the sketch, then it stays in that mode. There is already a discussion about this, perhaps even a tracker issue.

You can always switch it off and on again. That should enable the autoconstraints independently from previous states.