3d Curve Wrap

[Guest Ramzi Asfour]

I have a pretty challenging modelling problem. I'm throwing it out here to see what you IronCAD wizards can do...

 

please download the attched zip file for the relevant pics and ics files.

 

I have this 2D profile: 1.jpg.

 

I want to wrap the 3D curve around a Ø1.375" cylinder (this is not a symple 3d curve projection) to look like this: 2.jpg.

I can do this pretty easily in our CAM package with a simple command called "wrap"....and modelling in this CAM package is pretty cumbersome.

 

The final intent is to create a slotted cutout in the cylinder shape: 3.jpg.

The 3d representation you see here is the result of a CAM package simulation and is not an actual solid.

 

I've been playing with this for about 2 days now and can't seem to make any progress.

 

I'm about to try playing with the surface and sheetmetal commands to try to make it work.

 

NOTE: Redesigning the 2D profile is not an option...it is dictated by one of our customers.

 

RA

 

slot.zip

[B. Ludin]

I'm pretty sure this is not currently possible in IC. Othwise, it should also be possible to make cutouts from unfolded sheetmetal and then refold it (an enhancement that has been requested a couple of times in the past).

 

Beat

[Rick Dorrington]

Heaven's no. Not a stumper. Say it isn't so.

[tlehnhaeuser]

Ramzi,

I believe I did it for you. See attached file.

 

Basically it involved using sheetmetal tools as you suggested.

 

1._ I cretated a sheetmetal part with a .8125 rad Bend almost full around.

2. Used "Custom Profile" in sheetmetal and dragged on to flat portion of sheetmetal

3. Edit Custom profile to project your edges of profile

4. Finish

5. Slected cel and custom profile at intellishape level and used "Modify Affected Bends" and pick the bend to modify. NOTE: Will only work in ACIS mode.

6. Then moved profile intellishape so it totally was projected onto radial portion of bend.

7. Exported Sheetmetal part to ACIS (.sat) and reimported. Becuase you cannot use SM parts in IC to split other parts. Must be solid.

8. Once reimported filled in center portions with cylinder (grag from catalog) to make sm part "whole".

9. Then slected your 1.365" Part and this new SM part and split then using the Split tool.

10. removed the part not need and DONE!

 

Hope this helps

Tom

 

PS: I can figurue your part out but can;t figure out how to attache a file on this new forum. Any ideas?

Edited August 27, 2004 by tlehnhaeuser

[cborer]

Heres my version.

With Boolean operations.

Dimensions need to be modified.

Best

Carlo

Boolean.ics

[Guest Ramzi Asfour]

Carlo...thanks for your help, but your file basically has a straight projection of the profile on to the cylinder.

 

Tom...I'd really like to see your file.

At the bottom of the reply dialoge should be a section for file attachments. Click on the "Browse" button to locate and select your file...and then click on "Add This Attachment".

 

1.jpg

 

You usually have to wait a little while...when the file attaches you should see a marker for the attachment.

 

2.jpg

 

Hope this helps,

RA

 

 

[tlehnhaeuser]

Ramzi,

For some reason this Dialog option does appear on my reply dialogs. I will have to contact IronDudes about this.

 

download here:

ftp://ftp.ironcad.com/upload/sceneAAA.zip

 

Tom

Edited August 27, 2004 by tlehnhaeuser

[Chris Lohman]

Tom the attachment option doesn't appear in the "Fast Reply" box. If you click on the "AddReply" button then you should see it.

[Guest Ramzi Asfour]

Tom, that's ok...I got it to work. What can I say ?...I'm in awe of your bolt circle status.

 

I've attached the file if anyone wants to have a look. The process works...very creative, but it would be nice to do it without exporting/improting...

 

RA

 

hmmm...having touble attaching the file...the board won't accept it (seems like it times out on the upload). In any case, I'll put it on when I get a chance...

 

 

 

[B. Ludin]

Tom - I can't seem to download the file using your link (I guess the Irondudes have removed it already). Can you re-post it the regular way, I'm interested in it, too (I've tried to reproduce what you described but it din't work).

 

Beat

a mere sphere, but at least it rhymes... ;-)

[Chris Lohman]

hmm it won't let me attach a zip file for some reason

 

try this ftp://ftp.ironcad.com/upload/sceneaaa.zip

[tlehnhaeuser]

Ramzi,

I'm glad it works for you. Your right, there should be a tool for this since IC is almost there with its project 3d curve tool, add one more tweak to that tool.

 

Chris, as for the attach dialog box. I tried every reply option and none give me the opportuity to attach a file. What can I say. I would attach a sreenshot......but you know (hee hee)

Tom

[tlehnhaeuser]

Oh Yeah! Bolt Circle!!!!! Yippee! Thats fits me more than Sagitarius. Ha Ha

 

 

Tom, that's ok...I got it to work.  What can I say ?...I'm in awe of your bolt circle status.

 

I've attached the file if anyone wants to have a look.  The process works...very creative, but it would be nice to do it without exporting/improting...

 

RA

 

hmmm...having touble attaching the file...the board won't accept it (seems like it times out on the upload).  In any case, I'll put it on when I get a chance...

7393[/snapback]

 

[Chris Lohman]

AH our very first rank progession; congrats Tom lol. The next step is "I-Beam" at 1000 posts.

[tlehnhaeuser]

I-Beam is even better....the most appropriate would be PanHead (ha ha)

Tom

 

 

AH our very first rank progession; congrats Tom lol.  The next step is "I-Beam" at 1000 posts.

7404[/snapback]

 

[Guest EricFoy]

Ramzi:

 

This may seem a bit of an aside, but it seems to me that your customer gave you a kind of weird specification. I'm looking at it like this: What you're making is apparently a bayonnet fitting of some sort, which should properly be specified in polar terms. It has an entry with a given width with radiused lead-in, followed by a helical ramp section, with a given helix angle, followed by a straight section of a length which should properly be specified in angular terms, folowed by a detent, which might be simply called out as an overbite depth and radius (matching the pin on the mating device). In most cases, this pin is simply cylindrical, so a standard end mill would cut the slot nicely. This in my mind is the proper way to specify a bayonnet form. If it came to you in a flat layout form, then somewhere someone had to lay it out from its original cylindrical shape. My experience has been that engineers often don't understand these kinds of transformations well, and some double-checking with the designer would be in order. One can forsee a comment such as, "I don't understand... we used the same shape on the one-inch fitting and it worked great..."

 

Anyway, with a spec in the form I have suggested, it would be a much simpler shape to model. This is not to say, however, that your problem is at all irrelevant. Not long ago I was modelling a bayonnet fitting myself, and found myself thinking, "whoa, there's no way to do this in IronCAD!"

 

So I'm thinking what IC needs is two new intellishape types: 1. Cylindrical Projection and 2. Polar Projection. These would be a bit different in that the drawing surface would be either cylindrical or spherical in shape, and the means of constructing geometry on them would be a bit different since you would have to work in cylindrical or polar space.

 

BTW:

The way I ended up doing mine was to project the geometry onto a cylinder through a subtracting extrusion (after stretching the geometry first to simulate the unwrap operation). I then created a surface shape and thickened it to my desired cut depth. I then subtracted my thickened shape from the original cylinder. This worked for me because the cylinder radius was larger than the length of my unwrapped geometry. In your case it would require extra steps.

 

[Guest Ramzi Asfour]

Eric,

 

You're right...it is a type of bayonnet fitting. How the customer specifies it is really beyond our control. If I had my way, the cutout would just be an L-shape with a detent (without the helical section). Regardless of how the drawing is detailed, the desired shape is understood. I'm an engineer myself and I have no problem understanding the geometry or the cylindrical and polar coordinates/projections.

 

We've already been cutting the profile for a while, but we decided to try to tweak the cnc programs to obtain optimum cutting/tolerance conditions. The modeling/re-programming excersize had a purpose of introducing tool compensation to the cutter path as well as updating the programs from legacy methods to current methods/documentation.

 

I thought about the cylindrical/polar projection idea, but it's such a special scenario that I don't know if it would be very practical to have it in there. a single point.

 

Wrapping planar geometry around a cylindrical/spherical surface seems like a relatively simple thing to do, that I'm sure it wouldn't take the wizkids at IC long to add it in. Creating surfaces from 3D curves is already in there, so the geometry would not be hard to model after that.

 

I originally tried modeling this using a 3D curve and a 2D profile sweep. It seemed like the most logical tool to use at the time...I would just sweep a 2D profile of an endmill (rectangle) along the desired path.

 

Drawing the 3D curve path was a little tricky and the sweeping tool rotates the 2D profile for some reason. I'm sure I can get around to modeling this shape without using the sheet metal section, it's just that I don't really have the time to look into it deeply.

 

On an interesting note...I asked for the customer's solid model. They use Pro/E and it seems like they had trouble modeling the shape properly to start with.

 

RA