Sheet Metal Guy Blog

09 Jul 2008   02:51:09 pm
Evenly Spaced Holes
A lot of sheet metal parts require holes patterns to be equally spaced. There is a real easy solution to do this. First, I created a simple sketch with points to indicate the center of the holes or any other feature that you need evenly spaced. I set a specific distance from the end of the part that must be maintained. Your first instinct may be to dimension the centerpoints, as shown below. But when the part length is changed, the centerpoints are no longer spaced correctly. Rather than using dimensions, just create three construction lines. I changed the line color and thickness so that you can see that it is not just one centerline, but three separate lines. Then, all you have to do is Ctrl+select your three construction lines and add an Equal relation. Now, when the part length is changed, the centerpoints remain evenly spaced.
		Category : SolidWorks | By : SheetMetalGuy | Comments [0] | Trackbacks [0]
18 Jun 2008   01:15:22 pm
New Slot Sketch Entities in SolidWorks 2009
Back on Dec 4, 2007 I wrote a blog called Create a Slot in a Sketch. I was playing around with the SolidWorks 2009 Beta and noticed a new Slot sketch entity type. There are four types of slot sketch entities: Straight Slot, Centerpoint Straight Slot, 3 Point Arc Slot, and Centerpoint Arc Slot. To create a slot in a sketch, pull down the “Tools” menu and pick Sketch Entities – Straight Slot. If you take a close look at the buttons in the Slot PropertyManger, you will see numbers 1, 2, 3, 4. I didn’t pay any attention to these at first, but I soon realized that the numbers correspond to the order of the mouse clicks to create the specific slot. In the Slot PropertyManger, pick the slot type that you want. Click in the graphics area to set the center of the first arc. Then, click to set the center of the second circle. Finally, click to set the width of the slot. The Slot PropertyManager has an Add dimensions check box that will add dimensions to the slot automatically. Below the check box, you can see that there are two options, depending on how you prefer the slot to be dimensioned.
		Category : SolidWorks | By : SheetMetalGuy | Comments [1] | Trackbacks [0]
09 Jun 2008   01:18:38 pm
Unfolding formulas
I was sent several pages of unfolding information last week. Since we do say, “If you have a k-factor chart you would like to share with others, email to me”. Well someone did. I sat down with all eight pages and reviewed the details. While several pages are dedicated to calculating the Back Gage distance for the press brake, buried throughout each page is the standard formula for Bend Allowance. He probably doesn’t recognize it. But when you check the math, that’s what it is. I see this a lot. People will tell me they have their own formula and it is different. Yet when you break it down, it is still the standard formula. They may have filled in the Angle as 90 or unknowingly set the k-factor to 1/3, but the formula is the same. Here it is for those who don’t know it. Bend Allowance = Angle * (PI / 180) * (Radius + K-factor * Thickness) Remember we have a page wih these formulas. Here is a link: http://www.sheetmetalguy.com/bending-formulas.htm There are also a few pages to determine the minimum die opening. I found these to be interesting and did not see anything to say they will not work. What I really liked, was the chart of Bend Deductions. It is a classic. In the title block, it was approved 10-15-35, so you can tell how old it is. It covers 90 degree bends for a number of different thicknesses and radii from 1/32 to ½. Yes, they are shown as fractions. People did not have computers or even calculators back then. I did take my calculator and reversed the numbers to see what the k-factor was that they used. I was very surprised. It is always in the neighborhood of .5, sometimes bigger and sometimes smaller. But since the bend deductions are written to 3 decimal places, I kind of expected a different range for the k-factor. Well it does say “For Rough Work Only – Accuracy Not Guaranteed”.
		Category : Sheet Metal | By : SheetMetalGuy | Comments [0] | Trackbacks [0]
22 Apr 2008   02:41:17 pm
Custom Relief Type
When you create an Edge Flange or a Miter Flange which does not run the full width of the connecting flange, you have an option to specify a Custom Relief Type. This is the notch or relief where the flange ends short of the end of the neighboring flange. It offers three types of relief, Obround, Rectangle, and Tear. The default being Rectangle. Then there is another default. It is the ‘Use relief ratio’ check box. But what ratio? Where did this come from? The answer is really simply, the question is does it do you any good? The ratio is the width and depth of the relief notch divided by the material thickness, with a range of 0.5 to 2.0. And what good is this? Well maybe an old plasma torch could benefit from this to cut the notch, but a good laser will make a narrower notch and a punch is going to need to be a standard punch size. My boss never bought me a new punch just because the drawing called for a new size. So if this feature works for you great! I prefer to uncheck this box and specify the width and depth of the notch. Try it! When you set the notch type to either Rectangle or Obround and uncheck the “Use relief ratio’ box, the dialog changes to two edit boxes. One for the Width and the other for the Depth of the notch. Since I normally want a minimal notch I set the Depth to zero and the width according to the manufacturing method and material being used. The style, Rectangle vs Obround seems to be a personal preference, although the laser machines cut a real clean Obround style notch keeping the Width very narrow. One more thing. In the Miter Flange, the Custom Relief Type does not like a Depth of Zero. So you need to set the Depth to a small number, even 0.001 will work.
		Category : SolidWorks | By : SheetMetalGuy | Comments [2] | Trackbacks [0]
20 Mar 2008   12:01:08 pm
Miter Flange on 3 Sides
The Miter Flange is a great tool to quickly place the same flange geometry on several sides of your part. However, I often hear from users that they have trouble placing the sketch or getting the flanges on the sides they want. A recent note from one user says he can’t get it to place the flange on three sides of his part. It does all four sides with no problem. This is because the Miter Flange command is what I call unidirectional. Meaning it starts on the edge you select first and at the corner closest to where you selected that edge. It then works its way around the boundary going away from the starting corner. Confused? I was too, so let’s look at a picture. When you select the first edge to place the Miter Flange, SolidWorks creates an origin marker at one of the corners. The Miter Flange will be created on the selected edge, starting at the Origin marker. The next edge which I can select is then the bottom edge, not the top edge. The third edge would be the right side of the part. The only time I can select the top edge is when all the other edges are also selected. So the moral of the story is pay attention to which edge you select first to start the command. Don’t start your sketch on the middle of the three edges that you want.
		Category : SolidWorks | By : SheetMetalGuy | Comments [0] | Trackbacks [0]
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