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In-context editing. When to use it ,When not to.
- Thread starter gbonds
- Start date
It does affect assembly performance. And if not used in a linear manner, can cause the assembly to get stuck in a rebuild loop. I recommend only using it in situations where the in-contexted parts will not be used in any other assemblies. Also, if possible the incontext features should be placed on parts that are below the parent part in the assembly tree. This will prevent that loop. In other words, don't have a hole in your base part driven by a part that is inserted later (unless you can't avoid it). This will allow your assembly to be solved on the first run through. Otherwise it will take multiple passes through the assembly tree until everything is solved.
-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist
-Dustin
Professional Engineer
Certified SolidWorks Professional
Certified COSMOSWorks Designer Specialist
Certified SolidWorks Advanced Sheet Metal Specialist
This is the very useful tool when you ae creating the components with external references. For example would like to add some relations between geometry which belongs to different components.
I'm also using in-context edition of component instead of opening it in sparate window to safe a time for such operation.
Artem Taturevich, CSWP
Software and Design Engineer
AMCBridge LLC
I'm also using in-context edition of component instead of opening it in sparate window to safe a time for such operation.
Artem Taturevich, CSWP
Software and Design Engineer
AMCBridge LLC
gbonds,
In-context editing is a powerful design strategy, and a mindbogglingly awful strategy for long term document control.
When your design is done go through your assembly and replace the in-context geometry controls with geometry controls local to the part.
How to F*&k Up Documentation with Solidworks
[ol]
[li]Design assembly A consisting of parts[ ]B and[ ]C.[/li]
[li]Use geometry from part[ ]B to control the geometry of part[ ]C.[/li]
[li]Finalize[ ]C, check it into your PDM, and send the drawing and/or 3D[ ]model out for fabrication.[/li]
[li]Modify part[ ]B.[/li]
[/ol]
Note how part[ ]C reconfigures itself depending on whether or not you have assembly[ ]A loaded.
Once you finalize the design of a manufactured part, you are generally not allowed to modify form, fit and function. In-context design allows this to happen randomly, without warning.
ShaggyPE's warning about keeping a linear structure becomes a lot nastier when you spend more time you spend applying in-context constraints, especially if more than one person does it.
JHG
In-context editing is a powerful design strategy, and a mindbogglingly awful strategy for long term document control.
When your design is done go through your assembly and replace the in-context geometry controls with geometry controls local to the part.
How to F*&k Up Documentation with Solidworks
[ol]
[li]Design assembly A consisting of parts[ ]B and[ ]C.[/li]
[li]Use geometry from part[ ]B to control the geometry of part[ ]C.[/li]
[li]Finalize[ ]C, check it into your PDM, and send the drawing and/or 3D[ ]model out for fabrication.[/li]
[li]Modify part[ ]B.[/li]
[/ol]
Note how part[ ]C reconfigures itself depending on whether or not you have assembly[ ]A loaded.
Once you finalize the design of a manufactured part, you are generally not allowed to modify form, fit and function. In-context design allows this to happen randomly, without warning.
ShaggyPE's warning about keeping a linear structure becomes a lot nastier when you spend more time you spend applying in-context constraints, especially if more than one person does it.
RawheadRex
Mechanical
In general, I tend to caution people on the use of in-conext (or as some people call it "top-down") design for the reasons already stated above. Additionally, I prefer "bottom-up" design because that is how things get manufactured. Having said that, I do admit that "top-down" technique does have it's uses ("you have to know when to break the rules") such as when you need to transfer a hole pattern that cannot be easily calculated from one component to another. Even at that though, I tend to delete external references once I've achieved my aim.
Best regards,
Chris Gervais
Application Engineer
CSWP, CSWST
Best regards,
Chris Gervais
Application Engineer
CSWP, CSWST
Ditto to Drawoh. Nothing will run you into trouble faster, except maybe shooting your computer with a shotgun.
Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group
Matt Lorono
CAD Engineer/ECN Analyst
Silicon Valley, CA
Lorono's SolidWorks Resources
Co-moderator of Solidworks Yahoo! Group
and Mechnical.Engineering Yahoo! Group
rgrayclamps
Mechanical
Simple rules in my house:
In-context is OK and preferred for part(s) that are truely unique and are used in only one assembly. These parts need to be revised to stand-alone parts if later they are shared among multiple assemblies.
Standard/common parts must be stand-alone.
In-context is OK and preferred for part(s) that are truely unique and are used in only one assembly. These parts need to be revised to stand-alone parts if later they are shared among multiple assemblies.
Standard/common parts must be stand-alone.
I use in-context editing a lot during ideation and when all I am after is a pretty picture.
Dan
Dan's Blog
Dan
Dan's Blog
Drawoh,
A good PDM system like dbWorks will force you to revision anything touched by in-context relations so that modifying B will force a revision on C as well. If it is set up correctly manufacturing will never see the new revision/version of A, B, or C until they are released.
There are some types of product that are built to vary in certain dimensions intentionally for each customer. In these cases in-context can be a real boon if used with a design table.
In general, I am a make and break guy with these things though. When creating in-context I will frequently place driven dimensions up front to control what is in-context. That way when I remove the external relation I'll only have to make the dimension driving and I'm done.
In-context can also be locked so that changes won't propagate till it is required. I do this when I use a surface from one part to define a surface in another part. This is used when working in the land of swoop.
TOP
CSWP, BSSE
"Node news is good news."
A good PDM system like dbWorks will force you to revision anything touched by in-context relations so that modifying B will force a revision on C as well. If it is set up correctly manufacturing will never see the new revision/version of A, B, or C until they are released.
There are some types of product that are built to vary in certain dimensions intentionally for each customer. In these cases in-context can be a real boon if used with a design table.
In general, I am a make and break guy with these things though. When creating in-context I will frequently place driven dimensions up front to control what is in-context. That way when I remove the external relation I'll only have to make the dimension driving and I'm done.
In-context can also be locked so that changes won't propagate till it is required. I do this when I use a surface from one part to define a surface in another part. This is used when working in the land of swoop.
TOP
CSWP, BSSE
"Node news is good news."
kellnerp said:
Not good enough. I am talking about after the drawings are released to manufacturing.
In most manufacturing environments, you should not change form, fit and function of your parts. This especially should not happen automatically. Consider what happens when the drawing revisor is not the same person who did the original design.
If you want to change the form, fit and function of a part, you should copy out the drawing and model and save-as to create new drawings and models. You can go in-context during your modification process.
Actually, I go nuts with in-context design. If you are not allowed to do top down design in SolidWorks, I see no point in running SolidWorks. When I exercise caution at finalizing time, everything works fine.
Maybe you misunderstood what I was trying to say. With dbWorks, we release a document at a certain revision to mfg. We then go to work on it at the next revision. Mfg. doesn't see any changes because they can only see the revision that was released to them. dbWorks locks things down so if you want mfg to see only rev 1 then it doesn't matter what you do with rev 2, in-context or no in-context.drawoh said:
Any decent PDM system will take care of this issue by creating a new version of all referenced documents for engineering while holding the customer (mfg) to the released versions.
TOP
CSWP, BSSE
"Node news is good news."
- Thread starter
- #14
Thanks for all the input. That was the kinda info I was looking for(opinions and thought on the subject). I understand that there are many ways to "skin the cat" but learning what others are doing and why helps me make the correct decisions when I am working with a new design.
Hope for the best, expect the worst, never be disappointed.
Hope for the best, expect the worst, never be disappointed.
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