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Extruding from a cylindrical surface

Knolly

New member
Hey:

Hopefully there is a simple answer to a problem that has been bugging me recently. I have a part that i want to design that is going to need 4 axis machining to make.

I basically want to be able to engrave the surface of the cylinder all the way around the cylinder.

It's basically a part that needs to be milled into the face of a cyclinder, but as the tool cuts it needs to always be concentric with the axis of the cylinder. Assuming I'm using a vertical CNC mill with a horizontal 4th axis (or a 4 aixs horizontal milling center) the 4th axis is going to rotate the part while maching: the mill is only going to travers in the X and Z axii (not Y).

However, when I'm trying to model up this part, I need a way to get a sketch to "wrap" onto the face of a cylinder. I've used the wrap and project fucntions, but they don't seem to work properly. And when I extrude a sketch that's on the cylinder face, it only extrudes it outwards in one direction - I need it to extrude perpendicular to the curved surface (a cylindrical sketch). I also end up with lots of discontinuities and weird edges (sorry not a great description).

Did this make sense?

Any help would be appreciated - thanks!

Noel


Edited by: Knolly
 
I don't understand why the wrap command does not do this to your liking. I modeled an example and placed it on our ftp site: ftp.orthman.com. The example is textexample. It has a cylinder with a 6" diameter. The text is wrapped around it and all edges are normal to the surface. I have milled lots of text in this fashion using a turntable on our 3 axis mill. It turns out great.



Edited by: horstmannb
 
Your link is password protected. I had the same question and wanted to view your file.


If possible, could I see the example of your text wrap?
 
I PMed the password and username to you.

1. All you have to do is draw whatever shaped face you want the feature to go onto.
2. Sketch whatever you want to cut out or project from that face.
3. Exit the sketch.
4. Select the sketch from the feature tree.
5. Then go to insert, features and wrap.
6. click the face you want the cut from and change the various settings in the command and then click the check mark and you are done.
 
horstmannb said:
I PMed the password and username to you.

1. All you have to do is draw whatever shaped face you want the feature to go onto.
2. Sketch whatever you want to cut out or project from that face.
3. Exit the sketch.
4. Select the sketch from the feature tree.
5. Then go to insert, features and wrap.
6. click the face you want the cut from and change the various settings in the command and then click the check mark and you are done.


mind if I ask for a little more detail on this?


if I extrude a cylinder, which face do I sketch my cutout feature on? I tried all 3 faces and none of them would let me do the wrap feature


thanks!
 
If you extrude the cylinder from the front plane, sketch what you want to cut on the right plane or top plane. Then use the wrap feature and it will put it onto the curved face. By the way, it will do this on any curved face like a loft or the like.
 
The way I do it is like below;


1- I extrude the cylinder or loft from which ever plane I need,


2- Then I create a second and extend it to the edge of the cylinder I want to wrap the text on,


3- On the new plane, I create a sketch of the text I want, (Tools, Sketch Entities, Text) then press exit sketch,


4- I highlight the sketch and click on wrap (Insert, Features, Wrap), and then click either emboose or deboss, then click on the rounded face of the cyliner.


Click OK, and there ya go.


The only thing I have not figured out yet is how to rotate the text 180 degrees. Can anyone help me out?
 
Two ways to rotate text 180 degrees:


1) Open the sketch where the text resides, double click on the text, then click the upside down letter (mirrors about a horizontal line relative to the text) and then click the backward letters (mirrors about a vertical line relative to the text).


2) Open the sketch. If you've placed the text on a curve, remove all constraints on that curve (horizontal, etc.), grab an endpoint and drag it.


I hope this helps,


Peter
 
Peter, Thanks for the help, I kinda figured I could puch the buttons, but mine are not highlighted. Am I overlooking a step to make them available?
 
You need to associate the text to a straight line:

  1. <LI>Create a straight construction line, left to right (I think- you can always flip the line).</LI>
    <LI>Start your text feature, but select the line prior to typing the text. The text now "adheres" (for lack of a better term) to the line.</LI>
    <LI>The buttons should no longer be greyed. You can left, right or center justify the text, etc. If you remove constraints from the line (horizontal, vertical, etc.) you can orient the text by dragging the line.</LI>


Be sure to use construction lines; if you try to make a cut with the text you might into problems.


Peter
 
OK, I have hit another hitch. I can not get SW to wrap to a loft or a cone. I get a failure error that I didn't write down.


From earlier posts, I understood it was possibe to wrap to lofts.
 
If your loft has a circular cross section, the plane that you sketch the text on needs to be parallel to the tangency of the face you are trying to wrap to.

To create a plane tangent to the surface draw two lines on the top face of your loft, one from the center to a quandrant of the circle, then the next 90
 
I guess I am not understanding how to make the plane Parrallel to the angle of the cone.


I can get a line drawn that is parrallel, to the cone angle, I just am unable to make the plane.
 

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