Pad On Top of Dome

[criageek]

Hi all - I'm trying to re-create some plastic knobs for an old Philco radio I'm working on. What I have isn't exact, but I think it's pretty decent. But I haven't figured out how to put the raised pointer on the top. Any ideas? Also, to make the dome on top I just created a revolution but it isn't actually 'attached' to the rest of the body...I just made the bottom edge of the sketch at the same position as the top of the pad for the body of the knob. Will that work out ok when I export to an obj file for the 3d printer?

Drat...my fcstd file is too large to attach...is that because of the 45 occurrence polar pattern?

So here is a link to it:

https://drive.google.com/file/d/0B2i1fb ... sp=sharing

Thanks!

Rich

Oops...here is my FreeCad info:

OS: Ubuntu 16.10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.17.10232 (Git)
Build type: None
Branch: master
Hash: 3136b42830f6da733cef1cc649760b97a6cdc836
Python version: 2.7.12+
Qt version: 4.8.7
Coin version: 4.0.0a
OCC version: 6.8.0.oce-0.17

[Willem]

Hi, here is a model with a raised pointer on top. I do not think it needs any explanation. I did not make the final cut because that makes the file grow from 120 kB to 5Mb so indeed that pattern makes the file big

Schermafdruk van 2017-02-23 10-23-17.png (71.43 KiB) Viewed 2519 times

[criageek]

Thanks Willem! I appreciate the help I've been tinkering with FreeCad for a few months now but I'm still pretty much a newbie, so I don't understand everything you've done. But I'll experiment some before asking questions.

Rich

[criageek]

I'm going to have to break down and ask for help. I managed to build the pointer on top with Willem's help...thanks!

But I am struggling with making the grooves on the side using a sweep and a cut. I can always go back to using a polar pattern for a pocket, but the sweep and cut should make it more like the original knob toward the bottom where the base flares out. I've attached a FreeCad file containing just the body of the knob and the sweep. Now when I go to the Part workbench, select the revolution for the knob body, then select the sweep and click 'Cut', all I get are the lines where the cut should be...but it isn't cut away. What am I doing wrong?

Thanks,
Rich

[renatorivo]

Edit the Sketch002, make tangent segments and arch

philco-renato.FCStd

(67.16 KiB) Downloaded 28 times

prima.png (21.78 KiB) Viewed 2436 times

dopo.png (22.23 KiB) Viewed 2436 times

renato

[NormandC]

Hello Rich,

That's a very nice project (they sure knew how to build things in style back then!), and this knob is an interesting modelling project.

What I have isn't exact, but I think it's pretty decent.

It is except for a few oddities. For example you created your dome sketch using a B-spline - kuddos on maybe being the first to use this new Sketcher tool in a project . But your dome ends up being slightly pointed, which is not what I'm seeing on pictures of Philco knobs.

Using an arc which top end is perpendicular to the revolution axis would create a true hemispheric dome. Or, if you want to keep your B-spline, then the second control point from the left should be aligned vertically with the one lying on the vertical sketch axis. You can also apply a perpendicular constraint between the B-spline end point and the vertical line, but it's tricky to select the B-spline end point: you need to select it from the Elements widget, by first unchecking "Auto-switch to Edge" then set the filter to "Starting Point". You will need to delete the coincident constraint, as it will be conflicting with a point-on-point perpendicular constraint.

Also, the dome ends before the grooves, which is not the case when you see the picture. Creating the grooves as late in the design as possible prevents that, and Willem's method is a nice one. But since you're using a 0.17 development version, you could use an additive pipe from the PartDesign workbench, then use a polar pattern - so you wouldn't need to leave the PartDesign workbench.

But I am wondering if sweeping a circle creates a groove that is faithful to the original knob? It looks to me like it's a V groove with maybe a very small round at the bottom of it.

Also, the pointer at the top ends exactly at the perimeter of the knob rather than being shorter. Its tip is aligned with a groove tip. Of course, the question here is: how much do you want this knob to be realistic compared to the original?

See this image I found on the Net:


You won't mind if I post my own interpretation sometimes later?

Cheers,

Norm

[criageek]

Thanks for the suggestion renatorivo! I'll give that a try when I get a chance.

Thanks for the great input NormandC! I appreciate it. I know exactly what you're talking about on all of your points, and since my first posting I've tried several different methods. The one I've liked best is the one Willem used in his example...drawing the outline of the body and then creating a revolution. To me that looks like a very accurate representation of the body itself. I've been switching back and forth between 0.16 and 0.17 and lately have been working more in 0.16 just because that is more compatible with most of the tutorials out there.

I've seen the same thing you've noticed about the grooves...they seem more like a triangle with a slightly rounded point. I figured once I figured out how to sweep a circle to make these grooves I'd try to do it with a more accurate shape.

The image you posted appears to be from the website I found that offers a set of 4 of these for $20, which seems like it would be the right way to go. I don't know how I'd duplicate the pattern they have in the finish so mine would be plain brown. Although I'd have to check to see if they'd fit the shafts on my radio. My radio is a Philco 47-1230 (built in 1947 http://www.radiomuseum.org/r/philco_47_1230.html) and the website says they have them for '41 and '42 models. But this is a fun exercise and it would be really cool to be able to 3d print my own

Rich

[criageek]

I'm getting there! I'm not convinced I have the shape and depth of the grooves exactly right yet so I'll tinker with that some more, but I'm getting close!

In the attached FreeCad file I deleted the cut because it made the file too large. But if you download it, just select the Fusion then the Array and then apply the cut.

By the way, I finally found a decent way to count the grooves...there are 43.

Any and all comments/suggestions welcome

Rich

[criageek]

Time for a followup. My son-in-law finally received his new 3d printer this week so I went up yesterday and helped him put it together. We didn't get started until about 7:00 PM and finished assembly about 1:45 AM this morning. After a little sleep we did some initial tests and calibration this morning, made a test print, then printed a copy of the Philco knob. It has some flaws in the model that I need to fix (the ridges around the outside aren't deep enough and the shape needs to be a bit "sharper"...the overall height is close but the sides are a little too tall so the dome on top is a little too flat...and the opening on the bottom side for the shaft is too small) but otherwise it came out really nice. How cool!

IMG_20170311_175339_r.jpg (221.16 KiB) Viewed 2324 times

My 3d printer will be ordered tomorrow!

Rich

[NormandC]

Very nice!

That's one of the better things in CAD: seeing your virtual work made reality.

There's a topic about that in the Users showcase: From FreeCAD To The Real World, your Philco knob would fit right in!