Curving a slab

[rovernut]

HI,

I have a task to complete and I can't figure out how to do it so I'm looking for some help. I am very new to this and self taught so I apologize in advance if this is too simple.

I have a slab measuring 10mm x 40mm x 5mm (L x W x H).  On the top 10 x 40 face I make a sketch with some small circles which I extrude partially into the face to I have a few small circular indentations in the face.  I now want to bend this slab to a specific diameter so its essentially a curved slab that would say fit on your forehead.  I know the radius I need, I just don't know how to make the bend and keep the circular indentations on the now curved surface and not distort the circles positions.  I need the circles to be in a certain orientation.

If I draw a curved slab I then can't seem to make a sketch on the curved face to make my circles to make my indentations.

Any help would be really appreciated

Ken

[jeff_strater]

Unfortunately, there are not "global deformation" tools such as a general bend tool.  However, you can get there with a little work, and with "Project to Surface" and "Press/Pull":

first, create your bent slab:

sketch:

Then Extrude:

Then, create a workplane in the middle.  I used a Tangent workplane, but other types are fine, too:

Then, sketch on this plane, and draw your circles:

Then, exit this sketch, and create a second sketch (you have to create a sketch to project from one sketch to another).  Use the Project To Surface command:

select the curved face as the Face input, and your circles as the Curve input:

Make sure that "Closest Point": is the projection type.  This will wrap your circles onto the circular face.

Next, use Split Faces to imprint the wrapped curves onto the face.  Select the face as your Faces To Split, and a wrapped curves as the Splitting Tool

You can only do one of these at a time.  Repeat for the other circles.  Now, you have edges on your curved face:

Then, invoke Press/Pull, and select one of the imprinted circles.  Set the type to "New Offset", then CTRL select the other two circles:

Enter a negative value to inset the selected areas:

and the result should be what you expect:

Hope this helps.

Jeff Strater (Fusion development)

[rovernut]

Thank you for the very detailed steps. I'll try this tomorrow and let you know.

Ken

[dunderhead]

Jeff, thanks for step-by-step advice. The need for the second sketch was a real mindbender. (You'll run into: "Not support projecting sketch geometry into same sketch, please change the target sketch or geometry." if you don't heed this advice.)

Now I'm so much less baffled after playing around a little bit. I'd suggest logging as a UI issue that the descriptions of the projection commands are a tiny bit confusing. So instead of:

Include 3D Geometry

"Include edges, work geometry, and sketch curves into the current sketch"  

(which doesn't explain the fact that this is about catching stuff on the 2D sketch plane!!!!)

Project to Surface
"Project sketch geometry, edge, vertex, or workpoint to selected surfaces"

(which perhaps implies that the current sketch geometry is acted upon and that somehow something is drawn on a surface!!!)

Perhaps try:

Include 3D Geometry as 2D

"Include edges, work geometry, and sketch curves into the current sketch plane"

Include 3D Geometry as 3D
"Project existing surface geometry to selected surfaces as 3D geometry into current sketch"

With this naming it's made clear that both include 3D geometry into the the current sketch.  The second command is pretty amazing actually, especially when set up with the timeline.

[nickfabb]

 I would like to do a very similar thing except instead of circles I would like to do text, both extruding in, and embossing out.  Can you provide any tips/tricks?

[herzinj]

Hi nickfabb,

I think this video should help you out a lot with what you are looking to do.  Keqing walks though how to do embossed lettering with the text command inside of Fusion 360.  You can use the same methods to extrude and cut lettering as well.

You might also want to consider using a .svg file for your text.  Depending on the font that you are using, variations in letter size, curvature and other factors, sometimes importing a .svg will allow you more flexibility, and then you are able to extrude and emboss as discussed in the video.

Please let me know if this helps or if you have any further questions.

James

[nickfabb]

Thanks James, I've watched that video before. However, I want to wrap the text around the circumference, or 90 degress from the way he did it. So the text reads around the circumference.  Similar to the E Pluribus unum in the attached image...Thoughts?

[herzinj]

Hi Nickfabb,

I believe a combination of the video and the steps provided above should be able to do what you are looking to accomplish.  Check out the image below with something I was playing around with… I’m thinking about printing my own money soon!

You can easily wrap text around the coin either as a split face, split body or projected sketch (I used split body myself).  Now, you won't be able to use this to wrap text the entire way around the coin, but you could quickly set up additional construction planes around the coin to continue the text.  Depending on how much you want written (written? embossed...) around the coin will determine how many planes you would need.  I'm guessing that 8 would be the maximum number needed, but 4 planes could easily get the job done.  It would then just be up to you for spacing and making sure you don't include too much text on any one plane to avoid significant warpage of the lettering.  There might be some other ways to do this, but nothing I can think of that would be easy (like a pattern) to do with the changing text around the coin.  

Please let me know if this looks like it would work for you, and if you would like more clarification I am happy to create a Screencast of what I did.

Thanks!

James

[herzinj]

It also just struck me that you might want the fancy curved John Quincy Adams text on the top of the coin.  This is where the .svg file would come into play.  Programs like Adobe Illustrator can create this curved text (and probably others like GIMP) which can then be saved as a .svg file and imported into Fusion.  The same split face, split body or projecting can then be done to the top face of the coin!  As far as I know, there's no simple way to make this text bend in Fusion 360, without perhaps creating a large number of sketches.  I can ask around for simple ways within the product for this to happen though. 

James

[nickfabb]

Thanks James... This sound encouraging.  Is there anyway you can do the screencast for your "TESTING" example? I am very new to this and not sure how to connect the dots with new split planes, etc...   Also, I assume the "testing" can be extruded into the coin or out of the coin?

Thanks much!

[herzinj]

Hi Nick,

I think this should show you all of the steps for both extruding in and out of the coin. I tried to show a couple of ways to go about things, and there are also other methods, but these should be pretty simple to get you started.  Let me know what questions you might have!

[nickfabb]

Thanks James, I really appreciate the video. I follow what you are doing but I do have a follow up question. If I understand your method correctly, the created plane is tangent to the circle. In other words, each letter's extrusion is not pointed directly at the center point of the cylinder. Only the one letter that happens to line up with the center would be.  This would be most visible if you repeated the same letter. Each letter would each appear to have slightly different extrusions as you move along the circumference. I would like them all to be equal. Does this make sense?

[herzinj]

Hi nickfabb,

So what you’re asking for isn’t very simple, at least not as far as I can tell.  I have created another Screencast on an idea of how to do it, but I’ll call it a super-ultra-mega workaround, which could be a fair amount of work depending on how much text you have, as well as how many parts you want to do it to.  I will ask around to see if anyone has a better way to do this, but I THINK this should get you what you want, even if it is a lengthy process. 

Please let me know what questions you have.

James

[dunderhead]

This would seem like a perfect example for writing a little script! One interesting part would be the automated creation of 32 construction planes and associated sketches and then figure out how to center the ith letter on the ith sketch and select the resulting sketch face for ablative extrusion.  

I'd imagine the script would have as input the text, the angle per letter, the extrusion depth, a center point, an orbit plane, and an initial point defining the center of the first letter plane.  So the script would expect there to be two selected points on a selected plane when run and ask for the remaining parameters! 

I'm hoping that we'll start seeing more applications of scripting. There's nice documentation and the Spyder environment looks friendly, so I hope to delve into it myself.

[nickfabb]

Thanks James, that approach will definitely work. Too bad it seems like such a hack. I would have thought "simple" engraving around a cylinder would be a more common function and somehwat built in.  That said I can definately use what you have come up with as a great start.  

Thanks again!

[herzinj]

I’m glad to hear that this will work for you, even if it isn’t ideal!  I think (like mentioned above) that a little bit of coding using the API available in Fusion might make this easier for you.  Also, suggesting that this functionality be added to the software on the IdeaStation would be great.  I’m it would get a lot of support as a lot of people probably have applications for this function.

James

[nickfabb]

Idea added. Thanks for your help....

http://forums.autodesk.com/t5/fusion-360-ideastation-request-a/extrude-emboss-text-along-a-cylinder-...