deRabes Posted July 28, 2012 Share Posted July 28, 2012 Hi I'm trying to create a plane parallel to a tapered edge. I need this plane to create a sketch and use this to cut extrude the shape onto the tapered shaft as an inlay. All I can get is the default plane which is parallel to the axis only. Probably a pretty basic action but I need some help. Thanks Quote Link to comment Share on other sites More sharing options...
JD Mather Posted July 28, 2012 Share Posted July 28, 2012 If you don't already have a sketch line (used to create the taper?), then - Create sketch on plane perp to tapered edge. Project Cut Edges. Exit sketch and create workplane by selecting the angled line and the plane on which you created the sketch. If this isn't what you want - attach your file (or a representative example) here. Quote Link to comment Share on other sites More sharing options...
deRabes Posted July 29, 2012 Author Share Posted July 29, 2012 Hi Thanks for getting back. The file attached is an example of the part with which I am working. I need to be able to cut a groove in the curved area for inlay. I also need to be able to do this on a tapered surface. The parts are not generated by revolving about an axis but by a loft between circles. Any advice would be appreciated. ChanterHead.zip Quote Link to comment Share on other sites More sharing options...
JD Mather Posted July 30, 2012 Share Posted July 30, 2012 I'm going to be away from my Inventor computer for a bit - hopefully someone else will come along and follow up on this question. Quote Link to comment Share on other sites More sharing options...
Bishop Posted July 30, 2012 Share Posted July 30, 2012 I only have 2011 at work so I can't check out your parts, but ... based on the filename, this is extremely relevant to my interests. If I'm right, then "I've got Naill's" should make sense to you, DeRabes? Quote Link to comment Share on other sites More sharing options...
deRabes Posted July 30, 2012 Author Share Posted July 30, 2012 'fraid not, Bishop Quote Link to comment Share on other sites More sharing options...
Bishop Posted July 30, 2012 Share Posted July 30, 2012 Hm. A chanter, though? For pipes? Quote Link to comment Share on other sites More sharing options...
deRabes Posted July 30, 2012 Author Share Posted July 30, 2012 Yep. Ups actually. Don't get the "I've got nails" thing though. Quote Link to comment Share on other sites More sharing options...
Bishop Posted July 30, 2012 Share Posted July 30, 2012 Naill. David Naill is one of the bigger pipe makers, that's who made mine. Quote Link to comment Share on other sites More sharing options...
abstracted Posted July 30, 2012 Share Posted July 30, 2012 All you need to do is create a point on the tapered face. Then (with the workplane command active) click on the point, then click on the tapered face. In the image (i'm assuming I chose the right tapered face you were talking about), the top plane is just an offset of the tangent plane. You can barely see the point in the center of the bottom plane. Quote Link to comment Share on other sites More sharing options...
deRabes Posted July 31, 2012 Author Share Posted July 31, 2012 Hi I'm not sure this will do. The problem is that the plane does not follow the contour of the curve so if I create a sketch on the flat plane and extrude a cut into the curved surface as the inlay it will not follow the curve but will have high and low points. Quote Link to comment Share on other sites More sharing options...
abstracted Posted July 31, 2012 Share Posted July 31, 2012 I don't know what your inlay is, but I think this is what we're looking for? The depression has a uniform depth through the entire profile. Quote Link to comment Share on other sites More sharing options...
deRabes Posted July 31, 2012 Author Share Posted July 31, 2012 That looks good. Will it work like this on the curved section behind those flats? Also can I use this method on a tapered shaft section? Thanks again Quote Link to comment Share on other sites More sharing options...
abstracted Posted July 31, 2012 Share Posted July 31, 2012 Yes, you can do this for any strangely shaped face(s). There are multiple ways to do this depending on what your working with. 1) Start by making a plane that you will sketch the inlay from, it's orientation should be as if you were going to extrude the inlay into the model. Extrude the inlay (as a surface, not as a solid) so that it intersects the face(s) that the inlay penetrates. Use the split command to split the face(s) at the intersection with the inlay extrusion. Finally use the Thicken/Offset command to indent the inlay. In the following image you can see an example of the surface I am talking about Note (if you don't already know) that going with the thicken/offset command makes the offset extend in the normal direction at the edges of your profile. You can make the edges extend in an axial direction using a different method (Difference in next image). Quote Link to comment Share on other sites More sharing options...
deRabes Posted July 31, 2012 Author Share Posted July 31, 2012 thats great. I'll work on that. Thanks a lot for your help. Quote Link to comment Share on other sites More sharing options...
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