convert surface to solid body

[office6PUWT]

I am trying to extrude a number of curved sketch loops 5mm into a curved face but they were not closed. I patched them so as to create a surface but I can't fund a way to make them into solids so that I can extrude them. The attached image should make this clear but I've attached the file also.

many thanks Luke

[SharkDesign]

Lots of ways to do this. 

You can use thicken to 'extrude' them. (I'd use this method probably for 5mm.) 

You can make the entire extrude out of surfaces, then use stitch to join them and create a solid. (You can use combine to remove this material)

[JDMather]

First think I notice is several Unresolved Issues.

So then I went back to the foundation - Sketch1 and discovered that it is not fully defined?

Proceeding down through Sketch48 I found duplicate lines overtop of each other?

I tried to fix everything, but ended up deciding if this were my work - I would start over from scratch using what was learned from this attempt (and of course Sketch1 would be fully defined).

Corrected Sketch1.

No duplicated dimensions.

No extraneous geometry.

I would then proceed to Sketch2 and follow same rules.

[johnsonshiue]

Hi! Or, use Ruled Surface command (3rd option) to protrude the loop in a selected direction. But, the sketch has to be open or closed fully. Like JD mentioned here, the sketches have incomplete intersections or unclean intersections.

Many thanks!

[office6PUWT]

Thanks that was really helpful, I'm still stuck though on how best to model the levers which slot into the slits I've created perpendicular the the curved surround but also at a 30 deg angle? see attached screen shot and ipt attached also for you in the event that you can help.

all best

Luke

[SharkDesign]

You'd be better off modelling the whole thing as an assembly if that's what you're trying to make. 

If you want to do it in a part there's several ways to do it.

I'd probably draw all the keys as one big block, then use cutouts. Then add the rads on the ends of the keys. 

https://knowledge.autodesk.com/community/screencast/5a2a9059-4775-49fb-93d6-acf605f6e027

You might be able to draw one key and then use the pattern by sketch feature, but I'm not sure if it'll follow a curve like that as I've not used it much. 

But assembly is definitely the way to go.

[JDMather]

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@SharkDesign wrote:

But assembly is definitely the way to go.

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I would probably do as multi-body and then push out the assembly.

[office6PUWT]

Hi JD,

Thanks for taking the time to look over my messy work. I'm aware that this file is mess and I'm developing a series of bad habits as a result of the following issues with which perhaps you can help further.

1. Duplicate lines are a result of not knowing how to select a portion of connected lines or indeed how to combine separate lines into a single line

2. Also I do not know how to turn on mid point snaps so am double drawing lines from the halfway point

3. I also don't know how to select inidividual sides of a rectangle so am offsetting more lines than necessary when using this tool and then deleting the unwanted ones.

4. Is there a way (as in autocad) that I can select the line I want from  drop down of double drawn lines.

I've searched for hours online to find methods of doing these three things but have not found specific answers (perhaps because they are so fundamental in nature).

More widely, I have started by adding fx dims to my sketches but all too soon become lazy or run of out applicable terms by the time I've reach the 10th width. I'm also working from precise measurements which won't change so end up just adding the dims as I have them and ignoring my fx. I know this is bad practice but what use are parameters to me if I'm unlikely to want to change dims and their corresponding dims?

I was thinking perhaps there might be an iLogic solution to placing the 56 levels around the surround (there are all identical in shape but engraved with individual text flute, violin, solo ect...) I recently created an iForm to handle a set of expanding fans but my iLogic experience is rudamentary and as you've note my parametres are a mess.

I don't like creating files that are so messy but don't know how to tidy them up (ie delete an unwanted solid). I end up just wanting to finifsh and export the model into 3ds max from a file that is no use going forward which given the amount of time I've spent on it is a huge waste.

all best

Luke

[JDMather]

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@office6PUWT wrote:

1. Duplicate lines are a result of not knowing how to select a portion of connected lines or indeed how to combine separate lines into a single line

2. Also I do not know how to turn on mid point snaps so am double drawing lines from the halfway point

3. I also don't know how to select inidividual sides of a rectangle so am offsetting more lines than necessary when using this tool and then deleting the unwanted ones.

4. Is there a way (as in autocad) that I can select the line I want from  drop down of double drawn lines.

 1. Right mouse button Select Other for individual segments.  Extend lines rather than multiple and Combine (which doesn't exist).  When you run into trouble you should STOP and post question here rather than digging a deeper hole.

2. I don't understand this one - midpoint snaps should always be available.  Attach file here when you run into trouble.

3. I hesitate to reveal this one as it stays in effect even if you shut down Inventor and drives users crazy, but again, right click and turn off Loop Select to get individual segments (don't forget to turn it back on at some point).

4. See #1, right mouse button Select Other.  There is a lot of context sensitive stuff on the Right Mouse button (and Shift Right Mouse and Crl Right Mouse).  Right mouse button everything to find the Pro tip goodies.

Bottom line - ask questions early and often.  After a while you will pick up all the tricks, but if you wait till you've dug a deep hole... ...I remember when I was first learning Inventor I would come to this forum and pick up several tricks virtually every day for at least the first year or so, and then maybe once a week, then once a month...

Again, ask questions early and ask often.

[thangnguyenA75PU]

I want to convert to solid, what should I do? Please help!