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Making a box for the Mana board of my Plotter
ProApe
Member Posts: 125 ✭
Hello,
I would like to 3d print a box with a lid to house the Mana board of my plotter.
I have already got bogged down several times, mainly because there are connections on different levels for which I have to provide an opening in the housing.
One of the problems I encounter with the designer is the exact localization of the openings in the housing for the various connections.
I have designed the board schematically in Onshape, with its layout and connections.
What would help me to locate the openings in the housing would be if it were possible to make a projection of the connection on the board onto the housing. Is that possible?
Another problem: the onshape stop button, which is lower than the green PCB with the connections for the limit switches and also close to other elements, so I have to make a precise countersink with an opening.
This should be the only opening in the upper part, the cover, there should be openings in the housing for all other connections.
I have already tried to build the whole thing in various ways and always get bogged down.
What is the best way to approach such a project?
Kind regards
ProApe
https://cad.onshape.com/documents/36833c69a4c492904728b502/w/a9fa2b4ebaeb4852aca52f2c/e/2870f1073a4ed90d5a171e32?renderMode=0&uiState=684a92d3a0cd261959d9b9ee
Comments
The openings you wish to make can be precisely located by the Use tool in a sketch. As was done in the duplicated part studio in a copy of your document, sketches were created on the surfaces of the right and front sides of the box and with the Use tool the desired elements of the inner parts can be selected to create the openings. You have to tilt and zoom in close to target the desired elements. You can also change the view to Translucent to make selections easier.
The path I would take for this project would be, in lieu of using planes for part levels, creating the 3D parts, as you have, on one of the default planes either in the same part studio or each part in their own studio.
From there, create an assembly and insert the parts you have created into it. Fix one part. Using Fasten mate connectors, place the remaining parts relative to it. It would be very useful to create a Variable Studio which would enable the adjustment of the mate connectors to get the parts arranged to their desired positions without directly editing the mate connector. When satisfied you can, while in the assembly, create a part studio in context to create the box based on the assembled parts.
Some components, such as the Nano, may have already been modeled by one of the Onshape members or at an offsite source such as Grabcad which might be used in lieu of creating the model yourself.
The best way is to create a Part Studio in context of the assembly. There are plenty of learn.onshape.com references to "in-context"
(incidentally I just did exactly the same thing for a home project for a guitar effects pedal - aligning the various holes for jacks, connectors, usb port etc was very easy when done in-context)
Your methods are certainly better and more professional than mine, and you certainly have a better overview of the progress of the project.
In the meantime, before I have learned a better method,, I have continued with mine and have made good progress. Whether it fits is another question; I'll have to print a test piece and check the dimensions again beforehand.
At the moment I'm stuck on a fillet that isn't like the others and I can't figure out why.
Another thing missing, which I had drawn in the sketch but not extracted, is the support of the lid on the housing.
https://cad.onshape.com/documents/f3e9ecf294bf6effc1182384/w/58a7de6f34b5227d12fbc971/e/911b50f9ed83cc63e358cb1e?renderMode=0&uiState=684ae657065dea4d41c16da1
By using a fillet of 11mm (radius of the base wall corner +(2x the 2mm offset used) I was able to come close. I think the best approach would be to create the sketch for Part 5 based on (aka: driven by) the previously created part for an exact match.
I did suppress an extrude in the feature tree. Perhaps that is the missing object.
O, so administrators can change a user's project that he has linked and shared with the administrators?
That would be cool! But I don't recognize any difference to what I did. So maybe that's not the case anyway. That would not be cool!
I made the contours of the lid by offset from the case: first an offset of 0.2mm (maybe 0.1mm would be enough) so that there is some play between the wall of the lid and that of the case, then an offset of 2mm from this offset since the walls are 2mm thick.
I don't understand why there is this incorrect arc radius at one corner as the radii in the underlying sketch are correct!
because your fillet 1 has an incorrect radius
O, so administrators can change a user's project that he has linked and shared with the administrators?
Perhaps they do. I don't know. But that sure ain't me.
When mentioning suppressing an extrude, I meant that I did that in my copy in case perhaps you copied it.
About matching arcs, When I used the dimension in my previous post for the fillet, it looked to me as if the dimensions matched but there was a slight difference in the shapes.
If you want to check your parts for fit, you can take a peek inside with Section Views. If you take another look at my copy of your document, you'll find a couple of named views. - Scotty
"When mentioning suppressing an extrude, I meant that I did that in my copy in case perhaps you copied it."
I don't find your copy anywhere.
The link to my copy of your document is embedded in the text of my first response to your post. Click on the bold blue text: copy. - Scotty
ok, indeed
sorry
I generally have a lot of problems finding the right sketch to make a change as there are many sketches and extrusions.
Is there a special method for this?
To keep features (sketches, extrusions, sweeps, etc.) easier to navigate, you can keep them simpler and uncrowded by creating parts that are independent from each other in separate part studios. Look at your current feature tree and imagine what it would look like and how much easier it would be to navigate if you had separate part studios for the Platine and the Platine Jribbecke. The remaining two parts are closely related and one will be dependent on the other if Using edges, faces, sketches from the part already modeled. I would model those two parts in the same part studio.
Naming Features will make it easier to identify where you want to go for editing.
I realize the dimensions of your box is dependent on the arrangement of the Platine and the Platine Jribbecke. Those dimensions could be determined by knowing the dimensions of the Platine and the Platine Jribbecke and some math. Other options are available too. You may want to look into the Derived feature and In Context modeling for those methods.
Hello,
I managed to reach my goal in my own, certainly not optimal and somewhat chaotic way.
The only small problem is the question why this recessed level, which should allow to press the power button (part 5, yellow in the attached screenshot) cannot be connected to the cover, but wants to form a separate part.
I have (once again) started from 0 and have made an effort to name the planes, sketches and extrusions from the beginning.
However, this becomes difficult when it's only about small corrections at the end, which is why I haven't named the last ones.
E.g. Sketch 6 and Extrude 3 which are used to fill the 0.1mm gap between the housing and the lid, where the edge of the lid is interrupted because the missing part (the yellow one) is lower.
Incidentally, I wanted to continue the edge identically vertically and horizontally at this point, but I didn't succeed, which is why I only closed this unsightly gap on both sides.
I also made an effort to create some order by putting all the elements concerning the board in a folder, but with the incomprehensible consequence that many of the remaining elements have turned red because they seem to have lost the connection somehow (the connections that come to my mind): Use and sketches resting on other geometry), so I undid that.
I have often the problem with many sketches that external references are supposedly missing, I don't understand why, but I can still extract them.
You propagate the division into separate part studios. What happens in this case if I want to place the bottom edge of one part on top of another part that is in a different part studio and that I can't see at the same time? For example, I need to be able to project the power button of the circuit board onto this yellow part (Use) in order to determine the position for the opening in the yellow part.
As you have correctly recognized, the dimensions of the housing and the cover depend on the dimensions of the circuit boards and the placement of the connections that have to be routed through the housing wall. I measured them as accurately as possible, both to determine the size of the housing (I left 2mm between the sides of the board and the housing and on the narrow side where the flat cable is located that connects the board with the limit switch connections (Jribbecke) to the main board I left 15mm to give the cable enough space) and to determine the exact position of the openings in the housing for the stepper motors, the limit switch cables, the 5V connection and the USB connection.
So far I don't know anything about Derived feature and Context modeling which might make things easier. I'll have to have a look at it; contest modeling has already been written about here.
https://cad.onshape.com/documents/04bf28c53f093f604c7922b7/w/c4bf1bab8cb3a082a7bfdcc4/e/28d67a40ce0e53e8c86123e9?renderMode=0&uiState=684e9299082a9427eae16f5b
When extruding Deckel tiefere Ebene, you are trying to add it to the deckel. Because the wand has not yet been created, the 'add' cannot be successful because it is some distance away from the deckel. There is not yet any connection between the body created in the extrude to the deckel. Move the roll bar, which is at the bottom of the feature tree as in the image below (light blue), up to below Deckel tiefere Ebene to see what I mean. The fix is easy. Use the Boolean tool to unite the part created in Deckel tiefer Ebene to the deckel.
document