Thin Revolved Cut in Assembly

[jdg268]

Anyone ever try this? It works fine in a part, but not and assembly. BTW I'm using 2007 sp2.2

For example, I have a shaft that is a part, and a feature resembling grinding takes off a few thousanths of an inch. I basically have horizontal and vertical lines with a centerline, and I can do a thin revolved cut just fine.

But, when I try to do the exact same procedure in an assembly, I get an error. If I then try to edit the feature, I crash. Anyone else run into this? Sound like a bug??

Thanks

John Graham CSWP

Mechanical Design Engineer

 

[CorBlimeyLimey]

What error are you getting?

 

[Theophilus]

I'd recommend not doing that (not just because of your results, but that's a great argument). I don't like getting features strung out across parts and assemblies if there's any way to prevent it. However, I'll often define my revolve sketch in the context of an assembly and then make the cut in the context of the part--simply converting sketch entities I pick up from the assembly--nothing more.

The reason is that sketchy things like errors begin to happen, since the relations are a bit more fragile when formed in an assembly. When possible, I think it best to have each part capable of standing on its own (apart from the assembly) before releasing to production. Splitting feature locations like this makes that difficult/impossible.



Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe transcends reason.

 

[jdg268]

Jeff,

Thanks for your input. However, we're somewhat pigeon-holed. We have a blank shaft that is turned down in one location of our plant, and it requires a drawing. The shaft then goes out for grinding, requiring another drawing. You may ask why we don't just make another configuration and change various OD's. The reason is that we want to have a BOM for the ground shaft (calling out the rough turned shaft). In order to have a SolidWorks generated BOM, I need to have a one piece assembly. There are some other workarounds, and I may consider them--like having a separte configuration for the grinding, then bringing that into an assembly, and creating a drawing from the assembly.

But, back to my original question. I should clarify that I'm trying to make an open contour, thin revolved cut. It works fine at the part level, but errors in the assembly

CBL, the error I get is:

​

Try for yourself and see if it works on a part but not a one piece assembly.

Thanks


John Graham CSWP

Mechanical Design Engineer

 

[Theophilus]

My guess for the reason this cannot be done is a safety factor--since you're in the context of an assembly (technically), you'll not be allowed to make an open-profile cut like that--or you'd be in danger of wiping out other components in your assembly.

I'd recommend closing your profile with another three lines and it should work fine. (Any reason it needs to be open?)



Jeff Mowry

http://www.industrialdesignhaus.com

Reason trumps all. And awe transcends reason.

 

[JMirisola]

I've had problems with assembly cuts like this before. For whatever reason, you'll need to close the sketch at the assembly level. I don't know that it's a bug in as much a quirk.

Jeff Mirisola, CSWP
CAD Administrator
SW '07 SP2.0, Dell M90, Intel 2 Duo Core, 2GB RAM, nVidia 2500M

http://designsmarter.typepad.com/jeffs_blog

 

[CorBlimeyLimey]

Any reason why you are trying to use an open contour and cut-revolve-thin?

Do you get an error when using a closed sketch and normal cut-revolve?

FYI ... A BOM can also be applied to single parts, so you could create configs of a single part with custom/config specific properties which would populate the BOM.

 

[ctopher]

It would need to be closed. It doesn't know which direction to cut.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 02-10-07)

 

[jdg268]

Thanks folks,

CBL,
How do you populate a BOM with entries in config. spec. custom properties? It's not really a true SolidWorks BOM, is it?


John Graham CSWP

Mechanical Design Engineer

 

[ctopher]

If it's a SW BOM, it's a true SW BOM.

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 02-10-07)

 

[CorBlimeyLimey]

Add a column to the BOM
RMB click the header and select properties
From the BOM Manager select Column Properties > Custom Properties
From the drop down list select property
Click the Tick

 

[jdg268]

Thanks CBL,
After I thought about it for a minute, that's what I thought you were talking about. I'm not used to having that feature available--we just switched to 2007 a few weeks ago.

John Graham CSWP

Mechanical Design Engineer