How to design a plastic part that has been "stamped" or "pushed in"?

Jin

Hi,

I am not sure if  I am using the right terms here when I refer to "stamping", here is the original part that I am trying to reproduce (so that I can print a replacement for the broken one):

I tried several ways of doing it, but did not like any of them; my difficulty seems to be the way of how to "push in the plastic" like in the original part. I first tried to achieve this effect by extruding the inner part and then applying a chamfer. It kind of looked OKish optically from the top (top being the side that raises up), but controlling the dimensions via chamfer angle and distance was more of a guess-game, so clearly there must be a better way and chamfering is probably not it.

I also failed at getting the bottom side (the one that is pushed in) right. My attempts included offset planes, remove-extrusions and all sorts of Extrude add/remove combinations, but even the ones that more or less resembled the object correctly appeared hacked up and ugly in terms of proper modelling, which tells me that I am going about it the wrong way.

I removed my ugly hacks, but left the attempts with the chamfered top (which I am not happy with because the angles are not correct) so that you can see what I mean:

https://cad.onshape.com/documents/d297316d463eb7e7d28ce72c/w/62e188b4674ee6c8de0323b6/e/2b7d3475af7397e5ce7a82f6

Is it somehow possible to take the "main shape extruded" solid and just "push it in" into the chosen direction to simulate the effect of how that part has been manufactured?

What would be the "correct" or "better" way to model something like that?

Kind regards,

Jin

alnis

Whenever there is a part with some complex geometry and a uniform thickness, it's a good idea to first go with a surface model, then thicken it to form the final solid. Also, the reason why I did the move boundary and then the split/delete was to get a flat face to put against the print bed (I'm assuming you will probably print it "standing up" to make the layer lines less noticeable). Here is how I would approach modeling this part:
https://cad.onshape.com/documents/90f372635b2b1109a6ecbe60/v/c21048fe022532c632f01f9c/e/884627bef50295285c4c9d20


Also, it can be very helpful to import the photos you are working with into sketches to use as a reference.

Hope this helps!

Jin

Wow, thank you! Indeed I now see why my initial approach was doomed to fail, I ignored surface objects completely and only tried to work with solids. I will go through your model step by step and learn the new technique, thank you very much for your help!

Jin

alnis_smidchens said:

Hope this helps!

I was able to retrace your design steps, learned some new things along the way, so thank you again - it worked out really well!

alnis

Glad to hear it worked out well!

Also, I just remembered: if you're adding plastic snap hooks on the model, I like to use the snap hook custom feature to keep everything neat and to make modifying the hooks later easier:
https://cad.onshape.com/documents/90f372635b2b1109a6ecbe60/v/7f90896de228605a8de726e7/e/884627bef50295285c4c9d20


I also like to print the sub-section of the model with the hooks first to test that they won't snap off. To do that, you can add a sketch with a rectangle encompassing the hooks and a little bit of the surrounding material, then extruding with the "intersect" option. That way, if the hooks break off or otherwise don't work, it's easier to iterate and get them working without using up a lot of print material and time. Just make sure to print it in the same orientation as it will be printed in the final model since 3D prints are not uniformly strong/weak in each direction.

Jin

alnis_smidchens said:

Glad to hear it worked out well!

Also, I just remembered: if you're adding plastic snap hooks on the model, I like to use the snap hook custom feature to keep everything neat and to make modifying the hooks later easier:
https://cad.onshape.com/documents/90f372635b2b1109a6ecbe60/v/7f90896de228605a8de726e7/e/884627bef50295285c4c9d20

That is really cool, thanks for the hint! Luckily on this particular part the snaps aren't that important, so I just copied them from the original piece 1:1 and all fits really well:

alnis_smidchens said:

Glad to hear it worked out well!

Also, I just remembered: if you're adding plastic snap hooks on the model, I like to use the snap hook custom feature to keep everything neat and to make modifying the hooks later easier:
https://cad.onshape.com/documents/90f372635b2b1109a6ecbe60/v/7f90896de228605a8de726e7/e/884627bef50295285c4c9d20
I also like to print the sub-section of the model with the hooks first to test that they won't snap off. To do that, you can add a sketch with a rectangle encompassing the hooks and a little bit of the surrounding material, then extruding with the "intersect" option. That way, if the hooks break off or otherwise don't work, it's easier to iterate and get them working without using up a lot of print material and time. Just make sure to print it in the same orientation as it will be printed in the final model since 3D prints are not uniformly strong/weak in each direction.

Right, that's a good idea as well, I already do that, mostly because I tend to mess up dimensions

I found out that I actually have two different kinds of separators in my drawer and having learned the new technique I went on designing the second part. However it posed an interesting challenge, maybe you could hint me what the better approach would be to model that? The thickness of this second separator is not uniform, so a regular "Thicken" operation won't produce the desired result. Of course I can get away with having all of it at 2mm, but since I'm learning OnShape I'd be interested in doing it right.

The main body is 2mm thick, but then the vertical side walls that create this "stamped" surface are only 1mm strong and the "stamped" plane itself is 1.5mm thick. That last part is especially interesting, basically it means that it starts at 2mm from the main body and narrows down towards the end to lose 0.5mm in thickness.

Am I correct to assume, that I should try to model the whole thing using surfaces and lofts, or is there a simpler way? What would you suggest?

The current approach uses your how-to for the first separator (so everything in 2mm thickness):

https://cad.onshape.com/documents/3b9cb150d4af5c8fe93c361e/w/be943e3f38cffdbf111d4be1/e/6fd06440e13770827756a575

steve_shubin

@Jin


https://cad.onshape.com/documents/f8e913bca2d3889d1581ec33/w/a41755fb84c66df85d0045ae/e/bc4115550abc00ccffaf3a6b

Jin

steve_shubin said:

@Jin


https://cad.onshape.com/documents/f8e913bca2d3889d1581ec33/w/a41755fb84c66df85d0045ae/e/bc4115550abc00ccffaf3a6b

Ooh, interesting, this approach looks almost simpler than the original one. So what I learn is - try to think broader in terms of tools that are there. I have been focusing too much on a particular way which I thought I should take, while I should have taken a step back and thought it over again. So once I learned the surface-thickening way I tried to squeeze the second part in there as well, instead of looking at the whole thing from a new perspective.

I actually did not expect anyone to model it, just to hint me Thank you very much, @steve_shubin  !

alnis

I like @steve_shubin's solution a lot! It's very clean and simple.

@Jin, I think that you'll find that there are many ways to model any one part, and depending on what you have to model and what the design intent is, different tools will be best. One thing to be careful of is that you will get slightly different results from lofting a solid between profiles and lofting a surface and then thickening. Here is a document showing this (it's not too important in most cases, it's just something to keep in mind):
https://cad.onshape.com/documents/4e169a67b28e7d98e5df2198/v/c9721b8159d42fe9d0e460ab/e/5c72b194f3ca1130985515d3

The slightly thicker one (made by thickening a surface) has a thickness of 20 mm exactly, but the vertical edges of the end faces are longer than 20 mm. The slightly thinner one (made by lofting a solid between profiles) has a thickness of slightly less than 20 mm, but the vertical edges of the end faces are exactly 20 mm.

Jin

Interesting, thanks for the hint! So far I somehow got away without surfaces and it's also been the first time really used "Thicken", usually "Extrude" was enough for what I was doing. I guess it's a good exercise to actually replicate some parts where you have to match the original. I have no background in properly designing parts, so most usually I end up with totally over engineered stuff which is a product of my imagination :> One of the learning downsides being that its usually faster to tune the design than to find a way to actually model it exactly as pictured.

Couple of lessons learned here, thank you!