What are your most impressive tricks of solidworks, Please spread this question to more people.
It is better to list 5~10 tricks for others, we will accumulated more and more in future.
What are your most impressive tricks of solidworks, Please spread this question to more people.
It is better to list 5~10 tricks for others, we will accumulated more and more in future.
Rob Edwards wrote:
I don't think I've posted this one before..
Even if I have it's worth repeating.
Move Face can take a feature as input
So it doesn't matter what happens to your faces
You can further hack this functionality creating extrudes from the resulting bodies
eg
It's not so often that Solidworks gives you a bonus.
Really useful for fast concept work, and so far very reliable.
great stuff Rob Edwards ,thanks for posting!
Ooooh I'm feeling tricky today!
Maybe this one's obvious to others but I only just realised
When adding constraints to a Move/Copy Body you can move multiple bodies at once and pick and mix just the minimum amount of mates to do the job.
4 Bodies - Just 2 mates (the classic L)
HERE is a trick i would like to unlearn add a parallel mate that over defines everything, but you can still move it before that mate.
I thought it was just my imagination, but I always felt like parallel mates led to less stable behavior.
This is a nice one I always forget until after I've done a sketch which I then delete.
You can make Planar Surfaces directly from model edges (similar to a Loft or Boundary) or defining a plane
Really useful for splitting, when you need a trimmed surface, instead of an infinite plane
Scott Perman wrote:
I thought it was just my imagination, but I always felt like parallel mates led to less stable behavior.
I think you're right. I've learned to only use them to lock down rotation on a component that's otherwise completely mated. (If all Concentric mates had the ability to lock rotation that wouldn't be an issue, but it's too early in the morning to get my blood pressure up, so I won't say any more about it.)
John Stoltzfus wrote:
Glenn Schroeder - You can lock "All" Concentric Mates, or am I missing something... ????
You can't lock Concentric mates if they involve a sketch point, sketch line, or axis. The sketch point I can understand, since it still leaves a lot of degrees of freedom, but I see no reason you can't lock one that uses an axis or line.
You can do it with axes;
Dave Laban wrote:
You can do it with axes;
Apparently I misspoke. I just double-checked and it works with sketch lines also. I could have sworn it didn't when the Lock Concentric mates function was first introduced.
It's capabilities have been expanded over the years, I vaguely recall axes not working when it was first introduced. What version are you on? I just tried using a sketch line in 2018 and it didn't let me.
Dave Laban wrote:
It's capabilities have been expanded over the years, I vaguely recall axes not working when it was first introduced. What version are you on? I just tried using a sketch line in 2018 and it didn't let me.
SW2019 sp 3.
Scott Perman wrote:
I thought it was just my imagination, but I always felt like parallel mates led to less stable behavior.
I think you may be onto something, I only use to line things up, then dump in favor of more conventional mates!
Scott Perman wrote:
I thought it was just my imagination, but I always felt like parallel mates led to less stable behavior.
I'll use a parallel mate to orient the part, then I'll delete it, and lock rotation on the concentric mate. I don't know why, but parallel mates are buggy. I've stopped using them other than to temporarily position a part.
I actually have the opposite way of thinking, but my way of thinking comes from working with flexible sub-assemblies.
Concentric lock has caused us headaches with flexible sub-assemblies. When the sub-assembly needs to be flexible, I will use a parrallel mate. If it's an assembly that does not require flexibility then I would probably use concentric lock.
Parrallel mates can flip rather easily so it is imperative to put them according to something that cannot/should not flip, for example a plane.
Albert Griego wrote:
Scott Perman wrote:
I thought it was just my imagination, but I always felt like parallel mates led to less stable behavior.
I'll use a parallel mate to orient the part, then I'll delete it, and lock rotation on the concentric mate. I don't know why, but parallel mates are buggy. I've stopped using them other than to temporarily position a part.
About the only thing that I use parallel mates on is a plane to plane mate. I will mate one of the primary planes of my part to a plane in the assembly (or the ssp) that I want it parallel with to orient the part. I don't really use the lock rotation ever.
Reference Plane to reference plane parallel mates seem to be pretty stable. Its when you get into the realm of surface to surface or something similar that I have seen the bugs happen.
Dan Pihlaja wrote:
Albert Griego wrote:
Scott Perman wrote:
I thought it was just my imagination, but I always felt like parallel mates led to less stable behavior.
I'll use a parallel mate to orient the part, then I'll delete it, and lock rotation on the concentric mate. I don't know why, but parallel mates are buggy. I've stopped using them other than to temporarily position a part.
About the only thing that I use parallel mates on is a plane to plane mate. I will mate one of the primary planes of my part to a plane in the assembly (or the ssp) that I want it parallel with to orient the part. I don't really use the lock rotation ever.
Reference Plane to reference plane parallel mates seem to be pretty stable. Its when you get into the realm of surface to surface or something similar that I have seen the bugs happen.
I use lock rotation on fasteners, or parts like shafts. I don't like to have components that are not fully constrained, so I'll mate the shaft of a screw with a concentric mate, lock it, and add a coincident for the underside of the head. It works pretty good. I haven't had any issues doing that.
hi,i really want to learn to top-down modeling.but it seems it is not so convenient to do that in solidworks.i used pro/E before,and top-down is so good.i wonder if you could tell me how to use it better in sw,and if you have some materials or tutorials to send to me,that's best.many thanks.
and another question,i don't know the difference between top-down modeling and In context assemblies,it is the same for me.and my english is not so good.thanks.
Jacky,
Try searching the forums for SSP.
Also, I have a simple walk-thru in the PDF at Skeleton Sketch Part Method for Large Assemblies . IMO, you can't go wrong with SSP.
But, depending on what you are doing other methods can be quicker and just as robust, for example part in part.
I agree there is very little information available on top down. SW put out a thin book on the subject years ago. But there should be more.
not a lot of info needed. just a lot of understanding on how your assembly will go together. Then creating the equations and proper references to make the desired parts.
Sorry if i didn't read the whole pages of this thread, maybe some of my tips have been already said.
here is one (or a remind) : Fillet (basic feature)
but even me, I don't have the habbit of using it sometime... lol
we can switch a fillet into a chamfer / return to fillet / return to chamfer / etc...
but when "Fillet" is in chamber mode, we can't use an angle, we only have the Dim x Dim (for non symetrical).
It can be usefull sometimes, to avoid to delete fillet feature, and recreate chamfer...
Also a remind about "Mirror PRT" :
For near all the "mirror cases", many users think to create a mirror PRT, it need to put it in an ASM.
The ASM is absolutely NOT NEED !!
Just open the PRT, make sure there is a correct plane to do the mirror (or create it in the PRT).
Then just do : Insert / Pattern-Mirror / Mirror.
In Sheet Metal, it's better to use the "correct Fillet/Chamfer for Sheet Metal"
(and don't use the "basic 3D Fillet / Chamfer" use for geometrical volume)
Insert / Sheet Metal / Break Corner
And also, it's possible to swtich to "fillet <> chamfer" without deleting the feature !
it's just an option inside...
In this case I was wanting to recess the base from the top, with my top as the driving feature.
It's easy using Surface Extend to make a profile bigger, but unfortunately Surface Extend lacks the Flip Direction option available in Move Face, so this was a convenient workaround.