Help: Extrude cut using a circle with offset end points

Howdy every one,

Hope everyone had a great week. Thanks to those who helped me with my last task. This task is a little different. I hope someones game, if so, thanks for the help in advance.

I have a sketch on the bottom plane, and I need to cut multiple circles equidistant from each other, but here it comes... The end point needs to be offset by 45 degrees, making a diagonal cylindrical cut through the sketch.

I'm trying to make a scalloped fire selector for an AR15. I happen to have one, and I'm using my calipers to rebuild the switch. I figure, however basic my knowledge is, the best way to learn is start making stuff.

I'll export a jpg of what I have and I'll use illustrator to mark what I'm trying to accomplish. One sec...

So, that's the front plane, with an illustrator sketch overlay. I want to extrude cut through this object...

As always, your help is very much appreciated.

-Justin

Sweep cut circle along line path

or

Revolve cut of a rectangle

or

Loft cut between 2 circles.

How is it made in the real world? Drilled?

You might need to realign the circle perpendicular to the path.

Justin, chances are(as JD said) the holes are actually drilled through. As you have it drawn the holes would be an oval and really no good way to manufacture that part easily if a drill operation will do. You can use your diagonal lines there to create a plane. Using the Plane tool(on either the Feature or Surface tab up top) you can select one of the lines, then one of its endpoints. From there you can simply extrude-cut through your part and do a Linear Pattern of that feature. There are other ways to do it as well. With what you have there you could use the circle as your extrude-cut feature but just below the direction dialog box(where you select Blind, through all etc) there is a box to let you pick direction. For this you should be able to select your line. See attached file. It has both of these in it.

AngleExtrude.zip

Heya Shift and JD,

Thanks for your help guys. I unfortunately haven't been able to figure this out. The drawing I made was a little confusing. I thought about using the plane tool to draw a circle on and then extrude cut. Can I make a plane at an angle to the bottom plane? I'm sure I'll have to play with it a little. I really appreciate your help. I'll make another quick illustrator drawing looking at the bottom plane. The cuts aren't oval they are drilled through the switch. The ovals I made are confusing. I feel a little in over my head but I made it this far with nothing more than a finished product and a calipers.

Did you open the file i attached and look through it? I did it both ways for you in there. its a SW2011 file.

Did you open the file i attached and look through it? I did it both ways for you in there. its a SW2011 file.

Shift,

I did open your file. Thanks so much for that. It looks like you used the line tool, and made a line at an angle, and then made a plane normal to the line. Because the line was angled, it created an angled sketch plane where you made a circle, and extrude cut through all using the line as a direction. I'm not looking at it right this second, but the second option was you made a circle with a angle relation correct? I did notice your notes on the left, you named your features, thats a big help. I think where I'm having trouble is selecting the sketch to modify. I tried "editing sketch", but I might be using to many features at the moment. I'll definitely have to spend some more time figuring this out. It seems simple enough. Could it be because I have to many features? I noticed your sketches look thin/dim in the properties manager. Also, I keep getting this little blue funnel next to everything when I'm trying to edit or draw a sketch. Thats probably the feature manager filter right?

I'm at work right so I wont be able to report back any new findings, hopefully this evening I'll have some good news. Thanks guys.

-Justin

So a little reading brought up a solution to a question I had which was, how do I add a plane normal to an angled line.

http://youngdutchdesign.com/create-a-plane-perpendicular-on-a-line

After reading that, and inspecting Shift's example, I figure what I need to do is edit the initial sketch, while looking at the sketch from the side, sketch a new line at the angle I desire, and then using reference geometry select plane and select the end point, while making sure the plane is perpendicular to the angled line I sketched earlier. This should render a new sketch plane with the midpoint where the line and plane meet, thus allowing me to sketch on the plane and sketch the circles I wish to extrude cut through the sides of my little lever, exactly how Shift showed me in the doc he attached. This should go smoothly assuming features in play aren't interfering with my extrude cut. I have a sneaking suspicion that I may have added to many features. I chamfered and sketched on some of those features creating sub sketches. Hopefully they dont interfere to much. I'll report back later today.

Also, I keep getting this little blue funnel next to everything when I'm trying to edit or draw a sketch.

You have accidently turned on a selection filter.

Hit F5 and you will see a toolbar pop up with filters (probably at bottom of screen).

Click the left most icon to turn off filters.

You can hit F5 again if you want to hide the toolbar.

Justin, im not sure what you are seeing. The blue funnel i think you are seeing is the selection filter. You shouldnt see that icon unless you have a filter turned on. There are a few hot keys on the keyboard associated with the filters if you havent changed them.

The two options in this case that i would use are either the first option in my file with the plane created off the line. This allows some flexibility with the features, patterns etc.

The second option I would use is what JD mentioned about relvolving. The same plane the angled line is drawn on can contain a rectangle which would revolve around this angled line. This allows you to revolve-cut the hole without creating the plane or the extrude feature.

The 2nd thing in my file using a reference direction for the extrude I dont think is a good option here. The hole would be an oval and not round. I put that in there to show you it was possible but not practical.

Let me know if that does or does not make sense and we will try to get you going.

AWESOME!

Thanks guys! JD thanks for the heads up on the filters and the quick keys, Shift, thanks for the drawing.

You guys helped me out a lot! A while back I was talking about modeling some existing levers, and possibly creating new ones. I received a couple sample levers and I was stumped for a while. You guys have been a huge help.

I really enjoy working with Solidworks. I'm also really happy to have found this place.

Thanks again guys!

cool Justin, glad you got it done! Its a good feeling isnt it:)