Part in a Part; I don't get it... 1

[williedawg]

SW2006 SP4.1

trying to Insert a Part into a Part, then subtract the new body from the fixed one.

In this case, I have a #4 C'Drill that needs to "drilled" into the end of a small bar.

Someone suggested using the HoleWizard to do this, but I can't find any C'Drills in the selections. (maybe this came out in later versions)

I've read the Help section on Inserting a Part till my head hurt and still don't understand how the new Part is to be located by Mates...can't seem to complete the locating process.

If this is not the best method, can someone suggest another way?

Here's a screen shot of what's happening.

 

[JMirisola]

Rather than selecting the axis, select the round faces and create a concentric mate, then hit the check mark. Select the end faces, then coincident. If you wanted, you could also select a plane from each part.

Jeff Mirisola, CSWP, Certified DriveWorks AE
CAD Administrator, Ultimate Survival Technologies
My Blog

 

[mrf13]

Try picking on the two end faces and choose"concentric" as the type of mate. They should line up. If that does not work, then open an assembly document and then bring both parts into that... it is much easier to mate parts this way.

 

[handleman]

The temporary axis you are trying to select on the c'drill is "driven" by the cylindrical face of the c'drill body. That axis can't be generated until SW figures out where the face is. So you can't directly move the axis with a mate constraint, you have to use the cylindrical face to define the mate constraint.

Long story short, select the axis of the rod and the face of the c'drill to create the mate constraint.

-handleman, CSWP (The new, easy test)

 

[Eltron]

In the Hole Wizard Property Manager all the way at the bottom there is an option for Near Side Countersunk. Just check that and adjust your parameters. Much easier than what you're trying.

Dan

http://www.eltronresearch.com

Dan's Blog

 

[CorBlimeyLimey]

When the Hole Wizard was suggested, they were probably referring to the Legacy Hole hole type (second row - last icon). With this type you can select various hole styles, one of them being C-sunk Drilled which will do the same job as a centre-drill. Each of the Legacy Holes are fully customisable.

That is much easier than Insert > Part, mate, and Combine.

 

[ShaggyPE]

What are you trying to accomplish? Is it just a countersunk hole in the end of the rod? Or are you creating an animation where you need to show the tool doing the cutting or something?

If you just need a countersunk hole, use hole wizard without all the insert part stuff. Within hole wizard, you can change the hole types. There is an option to select a countersink for a #4 flat head (socket cap or machine screw) with three different fit options. This does work in 2006. It works all the way back to at least 2000.

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist

 

[CorBlimeyLimey]

If you go Shaggy's route, remember to change the angle to 60°.

 

[mncad]

Hi williedawg,

I got around all of these issues by using a library feature. I have a library feature with all of the sizes of centerdrills in it already. You just select the face that you want it on and pick the size. If centerline of the cylinder is on the origin all you have to do is pick the origin and the centerdrill is located, if centerline isn't on the origin create a sketch on the face you want the centerdrill and put a point at the center of the cylinder, then use that for locating the library feature. Attached is the file.

mncad

 

[williedawg]

actually, what I was trying to do was learn about Insert> Features> Combine> Subtract in general terms so that a "cavity" could be made by subtracting an inserted part from a base part by said process.

So, following the Help file re: the Combine>Subtract operation, something like a C'Drill hole seemed to be about as basic as one could get.

another example would be having a NPT fitting (no actual threads, just a tapered solid) and subtracting it from another part having a boss. (Yes, I realize that there's a Pipe Tap selection under HW.) Inserting a user-made "fitting" would give better control of the bulk of an assembly.

In the example given under the Help for Combine, there are shown 3 methods of Combine; however, Mating the bodies or parts prior to the Combine is not explained, so that's where I was at.

As to aligning using Mates in the rod/C'Drill example, I was able to get the C'Drill Mated to the axis of the rod by selecting the Surface as suggested by those above, but what I found out was that the Mate from the Vertex of the point of the C'Drill to the end Face of the rod (depth of cut) had to be established first. If the cylindrical face were Mated first, that Vertex would be buried in the rod. Of course the opposite exposed end Vertex could be selected, but that's not how DOC is spec'd out.

 

[CorBlimeyLimey]

When parts become buried like that, just change the display state to Wireframe or Hidden Lines Visible, then the buried end can be selected.

 

[williedawg]

OK, thanks Cor, I'll try that next time.

mncad, thanks for that file, that will save a lot of time.

 

[kellnerp]

actually, what I was trying to do was learn about Insert> Features> Combine> Subtract in general terms so that a "cavity" could be made by subtracting an inserted part from a base part by said process.

You can also create a cavity by putting both in an assembly and creating a cavity feature in the rod. The add/subtract/join is for creating geometry in a single part.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[ctopher]

I was thinking the same as kellnerp, try a cavity.

Chris
SolidWorks 09, CATIA V5
ctopher's home
SolidWorks Legion

 

[ShaggyPE]

gotcha.

I think for the purposes of trying to learn the functionality, you should try the cavity as well as the insert_part>Subtract method.

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist

 

[kellnerp]

... you should try the cavity as well as the insert_part>Subtract method.

I suppose using a part of a known shape to create a feature by adding or subtracting material would be a good method. The only danger is if SW changes how they do things in the future and somehow invalidates your work.


TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[ShaggyPE]

I definitely don't recommend using this method for the feature proposed. But for learning the functionality so it can be used properly, in an appropriate situation later.

-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist