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Tracing an imported drawing in Onshape
Hello,
I want to mill a stand for my monitor, I have drawn the shape on a sheet, scanned it and imported it into Onshape.
But it exists there as a separate tab and I don't know how to get the drawing into PartStudio to trace it in Onshape.
How can I do that?
Kind regards
ProApe
0
Comments
Create a new sketch on a plane. Then do Insert Image. Once that's in there, you can draw a line along the longest known dimension in your image, and dimension that line, which will scale the whole thing proportionally. Once it's sized and positioned how you want, complete the sketch and make a new sketch in which to trace (i.e. don't trace in the same sketch your image is in)
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Hello,
Basically quite simple!
I have traced the drawing with Spline and have 2 problems: the size is not correct and the curves are not cleanly traced (the template is not clean either; once I have understood the principle, I will trace the contours again as cleanly as possible).
How can I scale up the drawing and how can I trace the template cleanly in Onshape?
Kind regards
ProApe
https://cad.onshape.com/documents/9a78ee16677d61d5a4257964/w/be33da7c19e652541efee2d1/e/8967d807cf67bc86cee23b19?renderMode=0&uiState=681b5418719cf709ecdcf6f3
Ok, I remembered how to change the size, but I don't really know how to trace a drawing cleanly.
Hello,
I have finished the drawing, but I can't extrude the right part, the stand for the monitor (the left part holds the Mac Mini to prevent it from slipping and falling off the table, as it is very light), separately, although I can select this part of the drawing as a surface.
ProApe
https://cad.onshape.com/documents/9a78ee16677d61d5a4257964/w/be33da7c19e652541efee2d1/e/8967d807cf67bc86cee23b19?renderMode=0&uiState=681bb4c32754d0160f12c0e8
Are you looking for something like this?
https://cad.onshape.com/documents/83e708c3a499880499ea90a1/w/95c3fe641cd95bf35939ae92/e/b3c3270559f702afa919ae08
I think your main problem is that you are putting too much in one sketch. It's much easier to separate your design in different sketches and features. Also use different type of features like "thin" extrude or "shell" as well add fillets as features instead of putting it all in the sketch (see the part connecting the two halves: the extrude is just a rectangle and the fillets are added after).
You also have way more points than you need on the splines, which causes them to be "wavy" instead of being nice curves. I would also suggest read up on constraints to "lock down" more of your stuff.
Hello,
Thank you for your great work!
Yes, that's exactly what I wanted to construct (apart from the fact that there should be no recess for the monitor).
I've been told here before not to put so much into one sketch, but I didn't see how I could fit the parts of a coherent drawing/part into multiple sketches, and make sure they are coherent after extrusion and make a single part.
You did that in 4 sketches. I don't understand the purpose of the first sketch.
But why couldn't I extrude this surface, I still don't understand!
How can I get rid of superfluous spline points? If I want to delete one, I delete the whole drawing. And how do I recognise the superfluous ones?
There is a superfluous line in the drawing (see screenshot) that cannot be deleted. Why?
I am familiar with the shell function, I have also come across the thin function in tutorials, but I don't understand where I should use this function in this drawing, as everything is extruded to a certain height. So why replace the extrusion function with the thin function?
But now I don't understand anything anymore: since I didn't manage to extrude the right part last night, I closed onshape and went to sleep. Now I've just started Onshape again, with my original file, and the area that couldn't be extruded last night has suddenly been extruded as if by magic! Exactly as I wanted it. How is that possible?
Kind regards
ProApe
The first sketch is literally just the reference picture with one line added to be able to set the dimension. If you have a sketch with no external constraints, the first dimension you add scales the whole sketch:
Breaking things down in multiple sketches doesn't mean they aren't related, you can still add constraints and dimensions to elements from other sketches.
You've got some messy overlapping lines at the very top that are causing the issue:
If you select that tiny region it does work, maybe you selected things differently the next day and included that bit somehow…:
When working with splines, start with fewer points (basically the ends and one in the middle) and only add points if you can't get the shape you want by manipulating the existing ones. This is easily done by increasing the degree as required. even the way I did it isn't very clean…
This is probably a better way, doing one quarter of the shape at a time:
Not sure what you mean about not being able to delete the line or spline points, maybe you weren't actually editing the sketch?:
Using thin features or a shell is often easier to work with than using offset lines in a sketch. For example the area for the mac mini doesn't need the two contours. I'm only using the internal one here:
Many thanks for all the work you have done and especially for the (GIF?) illustrations!
As for the area on the right that was unruly the night before and wouldn't extrude at all, it was already extruded when I opened Onshape the next morning without having done anything. That really amazes me!
The thing about tracing physical drawings or shapes on photos is a tricky job that requires a lot of skill and practice. I had also tried Bezier curves, but that went even worse.
I had tried to make the recess for the mini with the shell function, but I couldn't make the walls 13mm thick and the floor only 10mm thick, but walls and floor only the same thickness.
"Not sure what you mean about not being able to delete the line or spline points, maybe you weren't actually editing the sketch?:"
I was!