-
In The Machine is the official blog of the Inventor Product Management Team. It is a way for us to share Inventor news, interesting information about successful Inventor customers and partners as well as tips and tricks. From time to time we’ll also use the blog to solicit feedback from users via surveys. This blog is hosted by Garin Gardiner our Technical Marketing Manager.
-
Remove Those Flat Faces
March 9, 2008, 10:38 PM Garin Gardiner
This tip is more aimed at those of you that create consumer products although I am guessing several of you that don't necessarily design consumer products will be able to take advantage of the tip. The other day I was designing something and needed to take a flat face and replace it with a slight dome. If you look at most consumer products, they often have close to planer faces although they often have a very slight dome on them that can be difficult to create. It is possible to use a "loft to point" to achieve this although I wanted a little more control. I ended up running across an interesting work flow that is very easy and gives me the look I often want. This tip has already found several great uses for me and I thought it might be of use to some of you. I will use this on a very basic box to give you an idea of the technique.
First I just create a rectangle and extrude it up to get a shape similar to what you see.
I then added fillets around the entire box using the setback option to give me a very nice rounded edges on the top surface. This will help my top domed surface look even better usign setback isn't required to make the dome.
From there I create a work plane offset from the top surface that has a small negative value so that it penetrates the box that we have created. The offset you use will depend on the size of the fillet and how high you want the dome. In my case I have a 1mm fillet so I will create a plane that is -.01mm from the top face.
the next step will be to either use the split or sculpt tool to remove the very small amount of material above the work plane. you wont see much of a difference but this will be more clear once we create the done.
Now that the excess material is removed we will delete the top surface which will convert our part from a solid body to a hybrid surface model that will allow us to create the dome we are looking for.
We can now use the Boundary Patch feature and select the open edge where the deleted surface once was. It will default to a "Free Condition" which will be planer just like the deleted surface so select the drop down and choose "Tangent Condition" to get a nice Tangent surface. For the following image I turned off the Translucency for the boundary surface so you can see it better.
We are almost finished! Now just select the Stitch command so that we can select the original extrusion and the new boundary patch surface to turn them back into a solid body.
It is very subtle at this point which is what I typically want although you can adjust the original offset plane with a larger negative value to create a higher dome. Lets take a look at the side view of our model to see what we have done.
Original Part
Part with dome
This is a very basic shape to show this although you can use much more complex objects to use this and get great results.
Let me know if you find this type of tip to be useful.
Garin
6 Comments | Add Comment In the Machine > Autodesk Inventor, Tips, Inventor LT
Comments
-
March 11, 2008 01:31 PM Kevin Sheehan
Great tip, I wlll be using this method tomorrow at work. Your fantastic tips have helped reduce I workload. Thank you
-
March 13, 2008 01:20 PM Warren Sweet
Garin, I tried it out and it works great. Thanks for the tip. Keep the tips coming, they are very informative and helpful.
-
March 14, 2008 03:39 PM J S
Thanks for the great tips! They save a lot of time.
-
March 15, 2008 11:48 AM Gerard Vernice
Really great tip. I have always found difficulty in achieving this particular shape. Thanks a bunch.
-
March 22, 2008 11:24 AM Gerard Vernice
As I said before it's a great tip; However I found a difficulty in dimensioning this curvature when brought in the idw. Any suggestions?
-
March 24, 2008 02:06 PM Garin Gardiner
Adding dimensions to a curve in the drawing environment is a little tricky. I would imagine you would like to add dims along a curve at a specific interval (like every 6 inches). If so you can place work planes at the interval you want (6 inches) and create work points at the intersections of the edge and work plane. These can be recovered in the drawing environment and you can add dimensions to the points. I realize this is a little bit of a pain and we are looking into a better way although for now you can probably get what you need.
You must be logged in to post a comment.