Rounded Beveled Edge with some confusing characteristics (at least for me as a beginner)

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I've posted a couple of questions on here regarding a Keurig Drip tray that I'm attempting to model for fun and practice.  The Drip tray is somewhat of an ellipse cut in half.  I'll post the part file of what I have, as well as some pictures of the actual part I'm copying.  So, my question is how to make this beveled edge that goes around the front of the ellipse.  I don't think I can just use the Chamfer tool because the offsets are different around the ellipse.  Towards the back (where the drip tray backs up to the Keurig Body), the offset is small, but in the front it is quite large.  I have no idea if this made any sense, but I hope the attatchments help you to visualize my problem.  Thanks in advance for any help! 

 

Additional Info: Solid Edge ST4 (Student/Education Liscense), Ordered Mode, I'm a beginner (about 3 weeks experience with the software)

 

I've attatched 3 files: the plasticdriphousing.par (which is the part I need help with), the metal piece that fits into it, and a picture of the drip tray. 

 

Thanks,

Brian Mixon

7 REPLIES

Brian,   I cannot open the file since it was created in a...

Phenom
Phenom

Brian,

 

I cannot open the file since it was created in a student version, HOWEVER: 

 

What I would do is draw a 2D sketch of the path the bevel will follow. Then, create a second sketch at one end of the path using the Plane Normal to Curve option in the Plane Step, and draw the profile of the bevel. Use the swept cutout command, define the second sketch as your profile and the first as your path, and it sweeps your cutout profile around your path. Assuming you have never used this command before, there are many things you have to do right for this to work. The 2D path you draw in the first sketch must be tangent continuous, the profile you draw in the second step must not leave zero-thickness edges, etc etc. 

 

(These instructions apply to ordered mode, by the way)

-Dylan Gondyke

Re: Brian,   I cannot open the file since it was created in a...

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Thanks for the answer. I tried using this method, but I kept getting some error that I think said the path had to be connected (which I had no idea how it wasn't), but I'll try it again tonight or tomorrow. I'll update on my results.

Re: Brian,   I cannot open the file since it was created in a...

Phenom
Phenom
Make sure that a corner of your cutout sketch (Sketch #2) is connected to the endpoint of your path (Sketch #1)
-Dylan Gondyke

Hi Brian,   From looking at your part at home [had to elb...

Esteemed Contributor
Esteemed Contributor

Hi Brian,

 

From looking at your part at home [had to elbow my way onto my daughters laptop, as has Student Edition loaded Robot wink] ...you would be better making this bevel to the part before making the "Thin Wall". The correct timing for some of these types of styling features is crucial.

 

The method I would recommend for you here is draw a sketch line on the right plane, at an angle [I set a dimension of 45deg] and make sure to place a connect relationship to the profile curve you already have on the top face.

Make a cutout, using a "Plane Normal to Curve" placed at the top end of the line....when the view is oriented, use the "Include" command to re-use the bevel geometry you have, but just use the inboard side, leaving an open profile to make the cut. As you can see from my picture, the part will now have a cut opening through the wall thickness, which you will need to address beforehand, by adding material below, or reducing the cut depth.

 

Also the sides don't appear to be tangent to the front, rounded area,...you may want to tweak that for a smoother result with the bevel cut also.

Sean Cresswell
Design Manager Streetscape Limited
Solid Edge ST10 [MP2] Classic [x2 seats]
Windows 10

Re: Hi Brian,   From looking at your part at home [had to elb...

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So, I should "Goto" the operation before I did the thinwall operation, and create my path, and cutout. Then use the sweep command to cut away the beveled edge. Then "Goto" the final operation in my Pathfinder. Is that about right? Also, regarding the sides being tangent to the front curved area... Here's how I got my initial shape: Due to the fact that the shape is not a circle, but more of an ellipse, I found the radius of the bottom curve by using and arc equation. I didn't really know what to do from here, so I measured in half inch increments up from the vertex of that bottom curved shape, and then measured out to the sides of the piece from each half inch increment. This gave me a branch going "up" and then lines going out to the sides to form some sort of a framework of the curve of the sides. I finished by using the curved line command by clicking on all of the endpoints of the horizontal lines. This isn't entirely accurate, but it gave me an okay shape of the curve. Is there a better way to accomplish the shape, but in a much more accurate manner?
Thanks,
Brian Mixon

Re: Hi Brian,   From looking at your part at home [had to elb...

Esteemed Contributor
Esteemed Contributor

Brian, actually, looking at the photo of the part again, there is not likely to be ANY straight lines to make the frontal shape, and could quite easily be started as an elipse protrusion, then cut the back portion off. [See attached]
Yes, the "GoTo" method is OK, one of the pitfalls of Ordered modelling though, is this reordering of features can sometimes remove the faces that subsequent features relied upon, and may cause a few errors to be displayed, and in the worst cases, failed features causing model degradation at those points. Usually easily fixed, with selecting "Edit Profile" and renewing the dimensions or relationships on the geometry.

 

KeurigPlasticDripHousing_SC2.jpg

Sean Cresswell
Design Manager Streetscape Limited
Solid Edge ST10 [MP2] Classic [x2 seats]
Windows 10

Re: Hi Brian,   From looking at your part at home [had to elb...

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Wow, how did I not think of the ellipse tool? Thanks again for your help! I'll probably have another beginner question in a few days, haha