I recieved another solution for the modeling task of creating end cut-offs in a tube that are normal to the surface. This particular solution was submitted by Charles Culp. Charles solution also uses surfaces, breaking down the process creating each surface separately. The key aspect to this solution is Charles use of a Ruled Surface to create the normal surface.
Ruled Surface Technique
Here is the SolidWorks 2009 file of the tube.
Cheers,
Anna
This was a question posed a few weeks ago on the SolidWorks Forums. How do you model a tube with an end cutoff normal to the surface of the tube? This is the type of cut that would be created with a laser. The tube is held in a chuck that rotates the tube around it centerline. The laser head will move along the tube centerline to make the cut. A google search on 'laser tube cutting' will get you several links to companies that do this type of work and have some neat videos of the lasers in action.
Tube With Trims Normal to Tube Surface
Using typical SolidWorks modeling techniques, Extrudes and Cuts with solid bodies, this looks like an impossible task. This is where we, as SolidWorks users, need to think beyond our normal tools we use everyday and take a look at some of the other tools SolidWorks offers us.
This type of tube is very easy to make using Surfaces. One of the cool aspects of surfaces is when you offset a surface it is offset normal to the seed surface. We can take advantage of this behavior to model our tube.
Surface Offset
What we will do is sweep a surface, then trim the surface and finally thicken the surface to create the solid body tube.
Tube Created Using Surfaces
Here is a video of the process and the SolidWorks 2009 file of the tube.
A very easy task when you break out of the thought process to create the tube with solids. There are all kinds of ways surfaces can be used to make your modeling projects much easier. In the future, I will explore a few other techniques for modeling with surfaces instead of solids.
Cheers,
Anna
Ever since SolidWorks developed a new way of creating Sheet Metal Forming Tools in SolidWorks 2006 with their Form Tools Wizard I have not used it. I use the old school techniques for creating the forming tool. The number one reason I do not use the wizard is the Orientation Sketch in the form tool sldprt file can't be edited and for my needs the Orientation Sketch created by the Wizard is inadequate for orienting the form tool.
Forming Tool Wizard Orientation Sketch Can't Be Edited
Old School Forming Tool Orientation Sketch Can Be Edited
I add quite a bit of construction geometry to my Orientation Sketch to help me with the placement of the lance tabs that I use for our carrier designs. There are 9 points that I can select to orient a lance tab in our carriers. I also add sketch geometry that outlines the size of the punch I am placing and the P0 (punch zero point/punch centerline).
It is important when placing our lance tabs to not have the punch bodies running into each other. If they do run into each other I have to stamp the lance tabs in two operations as opposed to one operation. Extra operations means more time and money is required to create the carrier. We try to avoid that whenever possible. Not being able to add this type of info into the Wizard Orientation Sketch is a huge detriment to the Form Tool Wizard.
Old School Forming Tool Orientation Sketch
Later when I design the tooling for this part, I also use the forming tool orientation sketch for locating the standard pockets we Wire EDM in the die, stripper and punch holder at the P0 (punch zero point) in the stamping tooling we create. I have the wire pockets created and saved as Design Library parts that I can drag into the tool models and anchor on the zero point of the form tool orientation sketch.
At the end of this post I will have a link to a zip file with the form tools and a coupon showing how I place the forming tools. The zip file will also contain a pdf of a typical lance punch we use, with the standard Wire EDM pockets that are in our tooling. From the pdf you should be able to discern my logic for creating the form tool.
Lance Tab Placement In A Typical Carrier
Lance Tab Placement In A Typical Carrier
In my carrier designs I create a Lance Tab Layout Sketch that I use to define the placement of the lance tab. After dropping in the forming tool, I use the orientation sketches in each form tool to locate (coincident, parallel, collinear, etc) to the lance tab layout sketch.
One key tip to keep in mind when using the old school method for creating form tools and orientation sketches is to not have any horizontal or vertical constraints within your orientation sketch. Be sure to delete any that are created and add the appropriate constraint to fully define the sketch. Horizontal and vertical constraints will restrict how you can orient the form tool in your model.
Here is a zip file which has SolidWorks 2009 files with a coupon demonstrating the techniques I use to place form tools. There is an old school form tool and a form tool created using the Form Tool Wizard. I also have a pdf of a typical lance punch we use.
Forming tools are a great feature in SolidWorks. Using the old school methods for form tool creation will offer you much more control when placing your form tools.
Cheers,
Anna
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