I'm a SolidWorks noob, unfortunately. Mostly deal with other modeling software.

Hi,
can you give more details about the problem?

Do you have a drawing or smth to show what you want to do?

hey guys, sorry it took me so long to get back. what I am really trying to figure out is how to place specific holes in the pieces I am designing using the hole wizard on solid works. when I try to create a point and get my measurements and then place a countersunk hole using the wizard it says I can't place a hole on an existing point. I am sure there is a way to do it, or a certain sequence I have to go about to be able to do it, I just have no clue what it is. any help or insight would be much appreciated!

I did figure out how to do the splined broach, and it worked out great!

I'm also new to solidworks, so forgive me if you knew this, but when I get that error, it usually means I need to put the part back into "sketch mode".

not sure how the newer versions of Solidworks are, but in the 2010 version, as soon as I plot the points I want to use as a reference for the hole wizard, and switch over to the features tab, it will only allow me to to do an extruded cut or a revolved cut while still in the sketch mode. I think I am just gonna have to settle for creating a circle in the sketch mode, do an extruded cut to the depth I want the countersink, and then do another circle and extruded cut through all to achieve the countersink hole I am trying to create. I can still do the pattern feature using that sketch as the template, but it sure seems like more work than it should be for a simple countersink hole. The program is fantastic, it's just figuring out all the quirks and proper paths in the build sequence.

Hi,
Did you try to go directly to hole wizard (without sketching the placement points) and place the hole approximately in their places, then exit the wizard and open the sketch under it and adjust the placement points?

I would simply create a plane to sketch a half profile of the countersunk hole then use a revolved cut to finish a single hole, then pattern the feature using the parts axis. Of course there are several other ways to do basically the same thing - start a sketch with a single circle, use sketch tools pattern for repeating the circle, then a cut through all, then do the same thing for the counterbore constraining the base circle to the original circle in the previous sketch, then cut with an offset from plan or offset from surface to control the depth of the counterbore.
I rarely use SolidWork's wizards because when someone comes in after me it is easy for them to see how the features were constructed using simple basic methods, rather than needing to know the idiosyncrasy of some of the wizards.
Hope this helps.

Glad to hear the OP sorted out the issue, but as some general SW and parametric CAD advice on best practices, as it is a sketch driven environment my typical work flow is this:
1. - Create a master sketch at the top level, with the key features you need (in this example locations for placement of the holes).
2. - Create a second sketch and convert the entities you need for the hole feature you need (or just convert the whole thing and only use the parts you need in the next step)
3. - Create a hole wizard feature and place the points on the existing points (they will snap and automatically to form coincident relations).

Note for this example step 2 can be skipped, but typically there is more than 1 operation you need to complete and sketches in SW are absorbed when you perform an operation, so best practice is to convert entities and create a second sketch.
Advantages of this method include:
- All changes being driven from the master sketch (or sketches if you have a more complex model) - this can be a huge time saver.
- Configuration variations become trivial, feature suppression and dimensioning is much simpler (particularly if you employ design tables).

FYI this approach works great in top down design for assemblies also - you can use the Layout sketch in SW if you want to achieve the same thing, but I've found it isn't really necessary.
Let me know if this helps anyone.