Solidworks piercing

[DWilliams1]

Need some clarification about piercing relation in solidworks. I am doing lofting and am not sure when a piercing relation is needed. Often it seems to not be available as an option. So, when is it available, and when is it highly recommended to use the piercing relation?

 

[CorBlimeyLimey]

I don't believe there is a hard and fast rule (there rarely is in SW), but fairly safe to say that if the option is available ... use it.

 

[DWilliams1]

Thanks, I know that Solidworks is flexible and doesn't tie you down, most of the time, to one method.

to clarify, part of my question is about how to use piercing? When is piercing available as a choice of end condition, only when doing a guide curve on a loft? How about on a sweep? I'm looking for clarification about when piercing is available as a choice in SW.

 

[JMirisola]

Generally, you need to be dealing with two separate sketches where the endpoint of the guide curve meets the sketch profile. Again, no hard and fast rules, more like guidelines.

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

 

[rollupswx]

If SolidWorks autoprojects the coincident relation when sketching you don't need pierce. If it doesn't, I prefer to first place a sketch point near pierce point and then add the relation. Then sketch will snap to the point when creating.

 

[TheTick]

Pierce is for connecting a point to a curve or edge that passes through the sketch plane, at the point where that curve or edge intersects the sketch plane.

Pierce does not apply to segments that are on a plane parallel to the sketch plane. Also does not apply to axes that are perpendicular to the sketch plane.

With sweeps, the pierce constraint will keep the profile sketch point on a guide curve.

 

[SnowCrash]

Generally, if you want something pierced that involves bone, you have to drill.

Oh, wait, nevermind, sorry.

--
Hardie "Crashj" Johnson
SW 2008 SP4
Nvidia Quadro FX 1000
AMD Athalon 1.8 GHz 2 Gig RAM

 

[mjcole]

rollupswx,

I'm glad I'm not the only one that uses that technique. I usually recommend using the pierce relation because if you are using a guide curve consisting of lines and arcs instead of a spline the pierce relation will occur for each entity along the guide chain whereas Coincident sometimes rem,ains on the start location of the original endpoint.

The one thing to be ware full of is that pierce relations can not be modified to associate to a replacement entity like a coincident relation can when dangling. I hope SolidWorks allows for this in the future.

The other nice thing about using sketch points is that you don't have to pierce an endpoint of an entity in your profile to guide its shape through the sweep or loft. they can be used to size the profile with Hz or Vt alignment between points or coincident relations.

Michael