I have an assembly with PartA and PartB. PartA has 12 configurations where it changes size. PartB is driven by PartA with a dependant sketch and a cavity fearture. I need PartB to have configurations to match the PartA configurations.
For the love of all that is holy please tell me there is a way to automate this as I have hundreds of these files to process
I inserted a part/body inside another part. Is it possible to replace it?
Another question: How do you update the external reference when there is a question mark?
You can replace body: Insert-Feature-Move/Copy function. For better understand you can follow this link – http://www.rickyjordan.com/2007/07/solidworks-20-1-2.html
External reference with question mark you must reattach. You can follow this link – http://www.solidsmack.com/how-to-fix-out-of-context-parts-in-solidworks/2008-02-12/
Hi,
usually we put the tolerance in the sketch or in the dimension feature (es. ± 0.1), to show in the drawing.
How can I capture in the DimXpert the tolerance assigned in my project ?
For example in my cube I’ve the L=100 ± 0.1, but if I use the ‘Auto dimension scheme’ or ‘Location dimension’, SolidWorks give me L=100 ± 0.5.
I find illogical to re-assign tolerance especially if I’m not the designer, but only the analyst.
Thank you.
Hummm I will have to test this to make sure I can replicate it but what you are saying could be a major problem. I would go to your reseller and report this to see if they can replicate it and if so then let SW know. If they cannot replicate it then there might be some problems with your files.
I have a question about positioning (moveing via the move/copy command) parts inside other parts.
I need to position a part with a flat face such that a specific point on the face is locked to a variable point in the part I am inserting it into. For simplicity think of it this way:
Take a cylinder, insert another part that is a cube. I need to position the center of one of the cube faces in the center of the cylinder a specific distance up.
Unfortunately I can not use an assembly because this is being used to create a subtract so (AFAIK) I can’t use an assembly.
One method is to simply make an assembly and then save it as a part.
There are mate commands in the Move/Copy Body command that should allow you to do what are trying to do:
I have yet to test it and how it would refresh withh the part in part mates but Brian is right. I would suspect thou that it has a 50-50 chance of working
I will have to try the assembly saved as a part thing. I don’t know if that will work given that we need it to update correctly and are using design tables.
I tried the mates in the Move/Copy body command but I could only get a corner or edge of the solid to mate to something. My problem is that I want the middle of a flat surface to mate.
Are you just creating multi-bodies in one part, or actually inserting a part in a part?
dang, no dice.
The problem is the ‘negative geometry’. In the example above I need to do a subtract taking the square out of the cylinder so I can’t save as a part because it converts everything to surfaces.
Still no luck with the move/copy dialog. I tried creating a point where I want to align to but it won’t allow that to be used for the move. I can get the vertical alignment right but not the horizontal alignments.
So we have in two dimensions a large circle with a point in the middle. And a smaller square. I need to center the square (which will change sizes with configurations) on the center point of the circle. But I don’t see any way to do that with the mates available.
I opened a new part and inserted two existing parts into it. I can then subtract one from the other but the positioning is driving me crazy.
Matt, one of the options when saving an assembly to the part is “All Components”. This makes everything save out as a body instead of a surface.
I just did what I think you are trying to do. You have to create Axes/Planes in the respective parts.
Then, instead of running Move/Copy, choose to Edit Feature on one of the inserted parts. Check all reference geometry needed for positioning under “Transfer” and check “Launch move dialog” under “Locate Part”. Do the mates there and you should be able to use the parts’ reference geometry.
Unfortunately, you don’t seem to be able to pull in Work Points… You can bring in sketches, but I can’t seem to be able to select a sketch point for mating either…
Matt,
You should be able to use reference planes and axes in a multi-body (part in a part) mate. They have to be selected for import during the Insert process.
Wait in a assembly have you tried to use the cavity function from mold tools with 0 offset it cuts the first part with the second. Would that not do what you want? Here is a video of how to do it I did a while back http://solidmentor.com/modules/mastop_publish/?tac=Tubing_Weldments
Looks like I have several things to try out. I will try all of these suggestions.
Thanks again all.
Matt,
First, in an assembly, Ben’s idea of using the Cavity feature in-context will work.
Second, the mates inside the single part will work, but you may need to split an L on the face of the part to create a vertex to mate to the other part. Use a Split Curve feature, and the corner of the L corresponds to the point you need to mate.
Doing this multibody is a clumsy workaround. The assembly should work better.
Ok I tried a couple of things:
* Saving the assembly as a part – This works but the changes to the original parts don’t seem to carry through so it is no good for my purposes.
* Creating geometry to mate with when inserting a part into another part – This is a horrible hack but it works, I got the whole thing up and running. Rather than using an L split I created excess geometry off the back where it doesn’t matter thus avoiding multiple bodies.
* Create a cavity – This starts off elegantly but I have a problem. The cavities do not seem to be able to be suppressed/unsuppressed by design tables. This creates a problem for my application.
I think I may just stick with using extra geometry to hack the mate into working when inserting a part into another part.
If anyone knows how to suppress the cavity features within an assembly with a design table please let me know.
You should be able to suppress and un-suppress the cavity feature like any other feature? If this is the case submit it to your reseller as a bug.
What would the syntax be? As far as I can tell I can suppress parts but the cavity becomes a feature of a part in the assembly. I haven’t been able to find any syntax for suppressing and un-suppressing a feature of a part in an assembly.
Maybe I just missed that in the help pages.
Scratch that – I figured out what you where talking about as far as suppressing and un-suppressing the cavities.
I will explore that method more.
CBL 2:08 pm on May 21, 2010 Permalink
Why not drive both A & B via a master sketch at the top level? Or (my preference) a master sketch within a ‘dummy’ part at the top level.
Ben 10:06 am on May 22, 2010 Permalink
Normally I would but I have a cavity feature that will not work with that. Thanks though
afee451 6:02 am on May 24, 2010 Permalink
For these situations I use a multi-body part to drive dimensions between parts instead of an assembly. depending on the specifics, you may not need the assembly at all.