I see a hole out there

Ah!  Spring is in the air! So many wonderful things all around us are finally making their way back: flowers, birds, butterflies, higher temperatures, tree top squirrels, gophers digging out my flower bulbs, those darn raccoons that keep messing up my yard…, and, of course, Little League baseball season! While sitting on the bleachers for a good two or three hours, I read from one of my books and watch my son and his friends practice their game, as well as their cheers. They have quite a few fun ones, but there’s one they seem to love, since they keep chanting it over and over. “I see a hole out there. I see a hole out there. I see an H-O-L-E, hole out there.” This intrigues me, you know? Where is this hole they see? What is it really they are talking about? Is it even a hole out there? I guess I’ll never find out! It’s not anywhere in my trusty manual “Baseball for Dum-dums”, and my son won’t say a thing! Anyway, it also gets me thinking about holes in general. More in particularly, about using sketches to place holes with the Hole Wizard. Why? Well, because it’s one of those useful speedy short-cuts that helped me when I took the CSWA and  it may help me again when, someday, I finally take the CSWP test.

How to place holes using the Hole Wizard was really hard for me to understand at first. I went through all kinds of trouble trying to avoid using the Wizard for that reason. It wasn’t until I saw how it’s done in one of Albert’s video tutorials, that it dawned on me that the position of the hole is determined by a point, a sketch, and that, as any other sketch, I can apply relations and dimensions to it just the same way. Now one thing to keep in mind is that the Hole Wizard can use both 2D and 3D sketches to place the center of the holes.  Basically, if you have a planar surface and you want to use the Wizard to place holes on it, then you want to use a 2D sketch for that purpose. In this case you need to preselect the surface before starting the Hole Wizard, otherwise, you’ll end up with a 3D sketch.

Using 3D sketches, on the other hand, offers an obvious advantage for when placing holes in non-planar surfaces, but they can be tricky to define, since several relations that are usually available for 2D sketches aren’t available for 3D sketches, and also because you have to be careful what you dimension your sketch from. It is always better to dimension from a plane or planar face, rather than an edge, vertex, line, etc. In the following image, the Hole Wizard was used to place a hole on the surface of the sphere. 3DSketch1 is the point that locates the center of the hole, and it’s position is dimensioned from  the front and top planes.

In addition to being able to define the placement sketch just as you would any other sketch in SW, there’s the added possibility of using linear and circular sketch patterns to place more than one hole. In the following example, a linear pattern was used to place a series of holes on this planar face. Notice how the entity to pattern isn’t the hole, but the point that locates its center. The procedure to do this is very simple: just preselect the face, activate Hole Wizard, choose the kind of hole you need and then click on the position tab, place the hole anywhere on the surface, and then deactivate the point command, to avoid placing any more holes.  Then you can proceed to insert the kind of pattern you need, linear or circular. The entity to pattern is Point1, the center of the hole you just placed there. Finish by dimensioning and adding relations to the sketch, just like you would any other one, and when you finish, click OK to close the Hole Wizard.

Just as a curious note, it is possible to do the same as in the image above by using the hole wizard to generate the first hole and then using a feature pattern to create the rest of the holes. The following image shows the same part, where the holes where created using a linear feature pattern, LPattern1. In this case, we are patterning feature, the hole that was created with the Wizard, and not the point that defines its center.

Both parts look just the same, but when comparing their file sizes I was shocked to find that the part where the Holes were created by using the Hole Wizard in combination with a sketch pattern more than doubles the file size of the part that was created using a feature pattern.  It’s 504 KB against 238KB! That is a big difference! I still think the Hole Wizard is useful, but, in order to keep my file size small, I don’t think I would use it in combination with sketch patterns if I needed to place quite a large amount of holes in a part.

Comments

[Mike Puckett]

Gabi,

240kb to over 500 kb is not that big of a jump in number, considering its approx 1/4 of a MB. While it did technically double the file size, in a more complex part, the percentage would dramatically drop. What I would like to know is which one rebuilds faster? In todays world where a 500gb drive is $100, storage is not an issue. Speed of opening parts, and rebuilding them is.

[Gabi]

Hi Mike,

Thanks for the comment! That's a good point I hadn't considered! I guess I should try the same experiment with a more complex part and check the rebuild time for both. It's hard to notice any difference in such a simple one.

[Gabi]

OK, this is my update. I tried a much larger patten with verification on rebuild on, then checked for the feature statistics on both parts. While the file size didn't seem so dramatically different this time (only 20% difference), the part that uses feature patterns does rebuild faster than the one using the sketch pattern with the Hole Wizard.

[Brian]

Gabi,

I have always heard that it is better to use feature patterns rather than sketch patterns.

I would also suggest that it is better to have your patterns at the end of the tree rather than dispersed throughout the tree (similar to the recommendations of placing all fillets and chamfers at the end of the tree).

Brian
http://www.cadfanatic.com/

[Josh]

Hey Gabi, this is great for two reason. First, it shows how you can really dig down into the specifics of how something is created, finding the best way.

And it also makes you ask, why should I have to be concerned with how I create a hole. hopefully solidworks is working on this with 2009.

I know I'd much rather enjoy modeling the part than concerned with which method is going to make it load faster, ya know. great post.