Turn a circular face into a dome

[Alastair]

Gosh, I ask for an answer and three people kindly send in a response!

First of all, this was very helpful to see where the relevant placement options are.

I have moved over the button to the appropriate place by shifting it 5mm.

I still have a bit of curiosity about a point though. If you look at my original attempt at the top of the post, where I used pads and pockets on the face of the base, I used construction lines with symmetry constraints to locate these features in the properly centred position. If I decided to resize the base, then the pad/pocket would move also.

1. The way the sketch is currently attached to the base, I will need to remember to update the placement manually if I change the size of the base. Is there a way to attach the new sketch to the base in a way that would resist size changes? I'm thinking that the way I applied construction lines to the face originally was probably the right tac, but then I'd have to erect that sketch001 at 90 degrees to the face somehow.
2. I guess this would go likewise for the placement of the construction line used for mirroring in TheMarkster's solution.
3. I need to cut a ring out of the bottom of the base as well to match the button above. I have used the pocket feature with external geometry. It looks like I need to do this for each side separately. Was there a sensible way to avoid this doubling up?
4. Using the pocket feature, on one side, I tried using the "type": "to first" option, which looked correct, but when I tried to "OK", I got this error about multiple solids. If instead i used the "type": "dimension" and put in the actual thickness of the base, it seemed to work. This method seems weak though as it would brek if I changed the thickness of the base? Was there another way to cut out this chunk?

pushbotton bottom 1.PNG (173.66 KiB) Viewed 567 times

One more question; I looked at the page that kisolre kindly pointed me to. It appears that this help page relates to the attachment of complete parts from the part workbench, or possibly separate bodies that were made with the part design workbench, rather than the attachment of a sketch to a face with part design. I might be wrong though?

Many thanks again

Alastair

[chrisb]

The way the sketch is currently attached to the base, I will need to remember to update the placement manually if I change the size of the base. Is there a way to attach the new sketch to the base in a way that would resist size changes?

You should thoroughly investigate the models uploaded. Try to rebuild every single step. In my model I used a reference to external geometry; that keeps things in sync unless you add or remove elements from the base sketch.

It looks like I need to do this for each side separately. Was there a sensible way to avoid this doubling up?

You can mirror pockets too.

Using the pocket feature, on one side, I tried using the "type": "to first" option, which looked correct, but when I tried to "OK", I got this error about multiple solids.

I'm not sure what you are trying to do, but if it is creating the hollow parts with another pocket, then the first face is the top of the domes which would leave the center posts as separate solids.

[Alastair]

You're right, I should have explored this Chris

I only found one model uploaded, which was your one. Indeed I see that it is resistant to resizing the base, such that the "bubble" will stay correctly located.

I've deconstructed your model as best as I can. I note that you shifted the initial sketch of the base to be centralised on the coordinate system and enforced with a symmetry constraint. This made parts of the design easier...

I also saw that on the underside of the base, you had a couple of identical and coincident lines that went between the two arc centres on either side of the base (sketch001). These were used as points to attach the centre position of the button/bubble onto.

I don't understand how they (the lines) were created though or why two were needed. I tried deleting them and recreating with "external geometry", but nothing was highlighted. I tried making everything invisible except "Sketch" to see if I could attach external geometry to that, but I got an error symbol (see picture).

push button construction line.png (670.4 KiB) Viewed 542 times

Could you show me how these lines were attached please?

[chrisb]

I had taken your model with the external geometry you used without thinking much about it. Now looking at it I would not reference edges from the Pad, but rather from the sketch. This increases robustness with respect to topological naming issues.

This is what I have done with the model attached here:
- when editing Sketch001 hide everything except Sketch
- remove all existing external geometry
- tilt 3D view so that you can see Sketch
- remove the point-on-object constraint of the left lower corner
- create an external reference to the horizontal line, I have moved the left lower end a bot so you can see how it looks like:

Snip macro screenshot-805fa3.png (17.59 KiB) Viewed 538 times

- create a coincidence of the left lower point of your sketch to the left end of the external reference.

- furthermore I replaced one of the 1mm constraints with an equality to reduce the number of dimensions used
- finally hide Sketch

[Alastair]

Hi ChrisB

Sorry it's been a while since you offered your last help. I've had no time besides my job, but now how some holiday!

Your help is much appreciated!

I've had another bash and am fairly pleased with the results... I've used your ideas to a degree, but your picture with the raised bit (for demonstration) gave me another idea of how to do the cut out at the bottom. So I have my designed piece now.

cateye part 3 image.PNG (156.7 KiB) Viewed 506 times

One thing I couldn't figure out properly. You will see I have cut out two holes in the base sketch that matches up with part of the revolution. I did this manually though by setting both to 2.9mm. I couldn't figure out how to tie the two together so that it only needed setting once.

I tried attaching points and construction lines to the x axis and to the bit of the x axis that radiates out from the centre of the circles on sketch, to see if I could create something to attach a constraint too, but I couldn't get these constraints to take hold. It was hard to select the relevant points for this. Do you have an idea how to do this last part (the existing solution is not so bad of course.

I have a further question, the expands from this but I may post on a different thread.

Many thanks

Alastair

[chrisb]

In this case you can use the seam point of the circle as an external reference. If the seam is at a different position you can control it by creating a circle from two arcs.

Another possibility is to use Expressions to transfer information about the radius from one sketch to another.

[chrisb]

Forgot the image. You can see that I removed constraints and moved the sketch. Then I added the external reference vertex.