I have a sketch which is in a plane that is at an odd angle incline (horizontal in one direction, but at an angle in the other direction).
I want to rotate the sketch plane so it is horizontal.
I can use the measure tool to see the angle (with a bunch of decimals), and I could rotate by the negative of that number, but that does not seem to be a good way of doing it.
Thanks.
Hi Peter
Select the sketch in the items list on the left.
Then press ‘M’ on the keyboard if that is still your short cut for MOVE.
Then drag or rotate the whole sketch with the Move & Rotate symbols, just like moving any object.
see picture.
Have fun, Arron
one way to do it:
draw a square on the arbitrary plane
make a solid of this and the sketch in question
make another cube on preferred base plane
select all on the arbitrary plane and then Align
choose an edge on both solid cubes
now Project the sketch on base plane
…not perfect but as you loose splines etc but the sketch is there with more than four decimals
But when I rotate like that, it rotates in 5° increments, and it does not snap to horizontal.
Is there some way to force it to snap to horizontal (even though the starting angle is something like 16.12345°)
If I project from the inclined plane to the horizontal plane, wont that result in a squashed result? Ie, a square would become a rectangle?
What BKE is describing this.
Use Align Tool
Use Project Tool to recreate the sketch.
If we could copy and paste angles within the app we wouldn’t need to do this.
We don’t have rotation snap based on main XYZ origin, but the starting rotation point of the model or sketch, that would be a new feature we need.
I usually write down the degree as note somewhere and just type it in manually, yes not very productive.
OK, so align the body first. Yes, that works fine.
Hopefully some way to align a sketch plane will happen at some point. Or snapping to horizontal/vertical perhaps.
Thanks
Thanks.
Actually I’m wrong there is a way!
I just remembered how I used to do it Solidworks. History Tree is so long I always avoided using it.
Select your Sketch and check your Sketch History. You can change planes.
This will affect your history downstream, extruded parts, etc… they will also change orientation.
That works well.
This didn’t matter to me since my objective was to get DXFs that I could laser cut from my various parts, and the best method I’ve found so far (including stuff I’ve learnt from this thread) is:
It’s more than a little tedious, but it works.
It’d be much nicer if there was an Export DXF from Face which basically did that sequence internally. For making laser cut objects, this would be a fantastic addition!
Thats a feature other have requested as well.
You could use the Drawing feature in shaper to export flat sides.
You could also use a unfold app like this one https://www.unfolder.app/
Its for papercraft but for getting flat dxf dimensions/math is the same and app is cheap.
I think that is what I tried and I found it extremely fiddly to get just the relevant face exported as a DXF.
Export Face as DXF would definitely massively improve the workflow, but I pretty much have the sequence down now so it is just tedious.
I did figure there must be tools that could take the 3D exported part and turn it in to a 2D DXF. But hopefully Shapr3D will add the feature since it has lots of other export options, and exporting for laser cutting seems a growing market.
The rotate tool is not limited to 5 degree steps.
You can type in what angle you want exactly, just click on the rotate angle number, then enter the angle.
Most of the time I just rotate to horizontal, then project on to a new plane on the axis.
I do this quite often as I regularly export DXF files to CAMBAM to produce the files for my CNC router.
An export to 2D DXF from a sketch or plane would be very useful and save time.
It would be extra useful if you could define which plane when exporting (xy, zy, zx).
Probably best if the origin of the export is either sketch geometric corner or centre.
Here are the steps to do the sketch output from an angled plane or face.
Please ignore Plane 01 in the pictures, it is not needed. Shapr3D will project on to the axis plane.
Step1: Measure the angle of the sketch to the axis you want.
Step2: Select the sketch you want in the items panel, then press ‘M’.
Step3: Start rotating the sketch in the direction you want. Click on the angle of rotation to display the manual entry popup. Enter you desired angle to align with the axis and select the tick.
Step4: Select the sketch, then the projection tool, now click on the desired axis plane. The sketch will be projected to the axis plane, and a new sketch number will appear in the item and history panel.
Step5: If you wish, you can now rotate the sketch back to where it was originally.
Step6: Select the new sketch in the item panel, select the isolate tool. Now export the DXF of the sketch.
I have included an extra picture to show the DXF opened by CAMBAM. All I did after import into CAMBAM was select the whole geometry and drag to align the centre with the XY origin. Note that the circle sizes are still exactly as entered in the original sketch. This shows that the projection to the axis must have been correct and perpendicular.
NOTE:
The Rotating of the sketch does not upset the history tree, even when you put it back. All that you will gain in history is the new sketch, unless you added a plane.
Yes, but the angle itself is a multi digit decimal. So even if I find the angle displayed somewhere and type in the reverse of it, there is presumably more digits not displayed.
Yes, this is basically the process I settled on, except I found that basing the created sketch on a face of a part rather than on the sketch gave better results - the DXF from the original sketch occasionally came out with extraneous lines and/or doubled lines which do not make it in to the projection of the actual face.
Hi there
I think you may be worrying too much.
If you rotate the sketch by what Shapr measures it to be, Shapr now thinks it is at the desired angle of Zero.
The measurements come out right on my CAM software for cutting on my CNC, and that’s what I need.
Ronald Reagan got it right “Trust, but Verify”.
If you look at the screen grab you can see that the top line is at Zero on the Z axis. If there was any error in the rotation and export from Shapr there would be a value other than Zero.
It will be nice if we get a 2D DXF output from sketch at some point.
However, a radius (fillet) tool in sketch is currently higher on my want list.
Here is the whole process up to export, as a video.
I know it is a manual input of the angles, but it works
I’m sure you’re right - given there is a projection on to the XY plane anyway, even if the sketch was out by 0.00001° it would make no practical difference.
That said, my aging feeble brain can’t reliably keep a 6 digit number rattling around in there reliably even long enough to perform this operation, so I’d end up having to write it does which is irritating (the problems of getting old (or perhaps an effect of covid) — I once memorised an entire shuffled deck of cards on a 4 hour plane flight).
Thanks very much for your help!
I am impressed, I can’t remember what I went to the shed for usually.
I always have a pen and notepad next to me when designing.
Have a good one
