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How to move a sketch with its part?
ProApe
Member Posts: 115 ✭
Hello,
If I move a part e.g. by -50mm on the X-axis, the underlying sketch remains where it was drawn.
If no changes are made to the parts, this is not a problem, otherwise it is.
Is there a way to move not only the part but also the sketch by a certain distance?
I have looked everywhere, but have not found the solution.
Kind regards
ProApe
P.S.:
I'm afraid I'm a bit too quick with my questions. Sorry.
This is the second problem for today that I have been able to solve myself. I'll look a little longer for the solution to the next problem!
It's quite simple: Transform, select the geometry and move it to the desired position. I had tried this before, but somehow I couldn't enter a value by which I wanted to move it, but only approximately by dragging.
https://cad.onshape.com/documents/001d0116c9ad6bb520d9fabe/w/b69a5873f1fdf4aee61f7f4d/e/e6e52b18581d250a8179511b
Comments
The more idiomatic approach is to design the sketch where you want it, then let the part regenerate. While I can imagine cases where it's convenient to not do so, that's still an antipattern that can be avoided with a better approach.
Ok, but that only happens if I decide to move a part afterwards, which is still not a problem because the sketch can stay in place. Problems arise when I want to change something on the moved part afterwards. It is quite tedious to re-extract a complex object.
It is certainly better to fix the sketch first, but you still have to have the flexibility to change something afterwards.
Can you link your document? The link in the first post no longer works. Transforming parts is not super common for everyday designing. You're not transforming in the Part Studio instead of using an Assembly Studio, are you?
I am transforming in the part studio,
I no longer have this document as I had linked it.
I have created a new situation where I have moved both the left and the middle blue part to the left, but the sketches remain in place, which totally contradicts my humble logic. As I understand it, they should stay together when the part is moved because they belong together.
By the way, the monitor sketch is red: "...did not regenerative properly. Some external references are missing".
I don't understand where the problem is and which references are missing; after all, the geometry could be extruded.
https://cad.onshape.com/documents/8091a5ec45ee20108ae5e77c/w/1d18af4074f1df94feedb931/e/0ef5022f66cb7100225bc056?renderMode=0&uiState=6845b67e18953b6f56e6133f
I would submit that that's exactly the desync here, hence Nick's point that transforming parts isn't very common. Parametric CAD doesn't provide a two-way relationship between parts and the sketches that produced them - it's all one-way top-down dependencies. If you want a part in a different place, the correct way is to move the sketch entities that produced it. That way, you avoid clutter in your feature tree, decrease regen times, and rely on the regeneration mechanism to do your work for you.
Really, that's the whole point.
Ok,
I have just drawn a geometric figure and extruded it.
Then I didn't move the resulting part but the figure in the sketch, and the part followed it.
So the solution is not to move the 3d object, but the 2d figure.
Yep, exactly. :D Change an upstream entity, everything downstream regenerates. It may take a bit of work to grok, but it's more powerful, in a practical way, than non-parametric modeling.
I looked at your document. Its the Mac Mini stand from the other thread.
It looks to me like you are just moving things around to see how they look in different positions with the transform? You should be using Assembly for that. Recommend you do the assembly training.
You said in your other thread you are CNC machining this project. These parts are not designed for machining. The end mill can't make those shapes. It looks more like 3D printing shapes.
Will you print/machine the 4 parts separately, then attach together somehow? If so, again, you want to be in asssembly.
If all 4 parts are really one piece, and going to be machined/printed out of one piece of material, then the part studio is the correct place to be. In that case, if you decide you need more space between the computer and the monitor the correct thing to do is to modify the sketch that controls that spacing. Not transform.
If things fail after you modify the early sketches, that's just CAD life. The better your get, the more reliable you will make the sketches, and you will anticipate to yourself "the spacing will probably change, so let me make sure the sketch will not blow up when this dimension changes".
One really good way to diagnose and fix your failures is to have a second browser window open at the point right before you made the major changes. To do this, make a version when things look "good" that you can later open in a separate browser window. Have the failed version on the left of your screen, and the old version on the right of your screen. Go feature by feature on each browser simultaneously to see what went wrong and fix. There is a training course for version control.
I think you took a decent overall approach, of making each main section a sketch with dimensions to the neighboring section, and then made the connecting portions separately. Doing it this way would make it robust when changing the spacings between the main sections (depending on how well the connecting sections were modeled).
Suggest adding a recess to the portion that goes under the monitor, so the monitor base fits into it slightly. This will keep the monitor from slipping relative to the base.
Finally, are you aware that Amazon sells Mac Mini holders that screw to the back of a monitor on its VESA mount screws for 20 USD? That could be an off-the-shelf solution for you.
Hello,
thank you very much for your very detailed comments and tips!
I have already milled the 5 parts (Mac mini, intermediate part, compartment for the backup hard disk, intermediate part, monitor stand) from one piece, without any problems, but only as a test from an OSB board; I will mill it in spruce wood and make some changes beforehand (e.g. the compartment for the mini is too wide and not high enough; I was limited by the thickness of the OSB board which is 23 mm I will use a spruce board of 37mm).
The connections are there to position the compartment for the mini so that it doesn't interfere with the monitor.
Your tip with the second browser window is good; I've been doing it so far by copying the workspace from time to time so that I can make changes to the new file that don't affect the original.
The whole operation is not aimed at saving a few euros (I live in Europe), but is a challenge for me in Onshape and an occupation for my milling machine, which doesn't work enough, as I use it purely as a hobby, or my 3d printer.