Hello, I am fairly new to Solidworks but have been 3d modeling for the last 25 years. I am trying to model a top-down assembly driven by a master sketch. I've created 4 different parts and the assembly using configurations. I can get everything to update correctly sometimes but it is not consistent. Will someone please look at my files and tell me what I am doing wrong. TIA Keith
Nice work. Config in Master. I haven't try that yet.
I have no problem with you file and Config in SW2019 SP4.
I do know SW does like Master Skeleton too much.
From what I can tell you've inserted the driving part into all of the driven parts. I'm not that familiar with that method. I generally add the driving part to the top of the ASM. Then I right click on it and the part I'm trying to drive and Isolate both, then I use relations back to the driving part in the asm to push external references to the part.
I am in no way implying that your method won't work, I'm sure it will. I just don't have much experience with it.
Hi Matt thanks for the reply. I'm not sure I follow.
You say "add the driving part to the top of the ASM". By that I assume you mean to copy the MASTER sketch to the top of the assembly, (ok, got it). Next you say "right click on it and the part I'm trying to drive and isolate both". Where does "the part I'm trying to drive" come from? Do I model a similar part, insert it and use that? How do I access the MASTER external references in the driven part?
Thanks for the help
It may not be problem with your method, I use the same, from Inventor.
It could be from SW config.
Sometime, after making changes in a file (part, assembly), you should go through each config and update them.
If not, SW might fail to update config when you active it down stream.
Config is powerful but sometime come with high maintenance cost.
Yes, exactly what I have been doing but it still seem to get stuck sometimes. I even went through the trouble to color code the different part configurations to help troubleshoot the model. I can see the parts changing color between configurations but there are times when the part will change color but the dimensions dont update. Just adding to my frustration. Ha.
Hi Keith
A couple of things I noticed
You have unconfigured dimensions that change between configurations.
Why SW allows that is beyond me, but I imagine it will cause problems?
eg
Also one thing I like to do is add a rebuild save mark for each config
2018 SOLIDWORKS Help - Generating Configuration Data
Good Luck
Rob
Keith Panik - Part in Part would be the best way to go "If" it would work and the same with configurations and design tables.
Let me explain...
Part in Part works for the initial design of the components, however, what I found was, if you want to make changes to the master part, with only the master part open and you need to add a new sketch or feature, the master part doesn't update in the initial components. There could be one way that it would work, (I didn't try it, just thought of it now), and that is using a sketch block, there is a possibility there, based on the work that Chris Scarlett has done.
Configurations work well in parts such as hardware and purchased parts and in some cases assemblies, however, if you're doing top down modeling and having those parts drive other parts in an assembly is not recommended, because to correctly rebuild the changes in the assembly, realistically you need to click and rebuild every configuration, the same happens when using a design table, you need to edit the design table and exit before the parts all rebuild properly.
The Skeleton Sketch Part Process (SSP), has the driving part in the top of every sub-assembly plus the main assembly. The key to using SW is to feed or push information down the feature tree, never pull information up the feature tree, this includes any sketches/planes or any other references used to drive parts. Doing it differently will subject your models to a performance drain called "Circular Rebuild"
Matt Peneguy - brought up a great point, "Isolate" - on of the most important part of the SSP Process, what this does is keep you from picking up on another component in the model, that way the component you're working on can be deleted and changed out without any errors popping up on other components, plus it's super simple and easy to do.
Master Sketch doesn't have feature, Sketch and Planes only.
It is part in part but no model or body.
Isolate as well as SSP.
Information stay in Master. Part can be deleted without affecting other parts.
All parts "mate" to Master only.
I usually put Master in assembly so I can Mate parts to it.
The goal is to make all Mates 0 in assembly.
Add a sketch for location of the finger.
This will remove your Global Variable.
Matt think MS create and use a body like SSP.
MS only use Sketch in "derived" parts.
Frederick Law wrote:
Master Sketch doesn't have feature, Sketch and Planes only.
It is part in part but no model or body.
Isolate as well as SSP.
Information stay in Master. Part can be deleted without affecting other parts.
All parts "mate" to Master only.
100% correct, but there are rebuild issues with part in part...
Test....
Add sketches & planes and see what happens..
Keith Panik wrote:
Hi Matt thanks for the reply. I'm not sure I follow.
You say "add the driving part to the top of the ASM". By that I assume you mean to copy the MASTER sketch to the top of the assembly, (ok, got it). Next you say "right click on it and the part I'm trying to drive and isolate both". Where does "the part I'm trying to drive" come from? Do I model a similar part, insert it and use that? How do I access the MASTER external references in the driven part?
Thanks for the help
I think John has cleared a lot of this up, but I'll add a few things. To start I create the asm, insert a new part, click on the front plane (I think you can click anywhere in the view but I always click the front plane because that's how I learned). That part has an Inplace mate added that orients it to the assembly planes and origin. If for whatever reason you lose this mate, mate the origin of the part with the origin of the assembly with the "align axes" checked. This first part is my SSP and will drive everything in that assembly. Then each additional part I add is mated the same. But as John pointed out I use Isolate to work in the asm and push references around. I have a walk-through example in the pdf over at Skeleton Sketch Part Method for Large Assemblies that should take about 20 minutes that covers the basics.
One key take-away is that you are working in place, modeling things where they are, not around the origin. This takes some real time to adjust to, but the benefits come at the end of the project, when inevitably a manager comes in and changes a dimension that would destroy a bottom up assembly (but I'm sure you know this, because you are looking into top-down).
This method is very scalable as long as you are careful and follow some basic rules...I think the biggest rule is to only push a reference down one level. Each subassembly has it's own SSP driven by the SSP above it. It's all explained in the thread above and the PDF, if you are interested.
Do that every day.
No problem.
Usually I create empty MS.
Create Master Assembly, insert MS.
Insert customer part into assembly.
Edit MS in assembly. Create Plane from part. Sketch, covert entities.
Exit edit.
Edit MS add sketches, plane etc.
Frederick Law wrote:
Do that every day.
No problem.
Usually I create empty MS.
Create Master Assembly, insert MS.
Insert customer part into assembly.
Edit MS in assembly. Create Plane from part. Sketch, covert entities.
Exit edit.
Edit MS add sketches, plane etc.
Then I'm doing something wrong and need to be educated - could you upload a simple assembly, that has a few sub-assemblies... It has been a few years since I tried it, guessing 2016 - 2017 sometime and everything worked well till they asked me to make changes and additions. So when I opened up the master sketch and added what I needed, the master sketch in the already modeled components didn't reflect those changes. I wanted to do Part in Part modeling for a long time, but every time I tried it the updates didn't rebuild cleanly. So I'm going to say that I'm not doing something right and need to be corrected by a FLaw - hehehe
I'll work something out.
MS doesn't work well in 2005. It had improved.
I need to try SSP also.
Maybe combine the 2.
I know it update because every time I add a new plane and sketch in MS, I need to hide them in every parts in the assembly.
The problem I have now is SW will duplicate Sketch in derived parts, after I edit the sketch in MS.
Thanks.
I'll turn on "Add Rebuild on Save mark to new config" in my template and see if it helps.
Ok..
Testing from my end..
While in part - can not change the dimensions (Driven)
Open the SSP and adjust dimension
Rebuild & close
Model Part Updated as it should have
Now add another sketch and part
The assembly
Modified Length
Closed assembly and edit the SSP
Open the Test Assembly
Changed the Profile
NICE - Another go on a "New" project (coming soon)
Thank you for letting me know that this is working, it's been a while since I've tried it, SW made some changes sometime..
when creating top down assemblies I would not use configurations. I would make each one a part and to make a new instance that i wanted to build I would do a pack a go on the drawing and then get a new copy of all the parts and assemblies associated with said drawing to a new folder, with new file names,
So now you have the same part in multiple locations with multiple file names? That would be a recipe for disaster in my world.
Scott Perman wrote:
So now you have the same part in multiple locations with multiple file names? That would be a recipe for disaster in my world.
Absolutely, for sure in a lot of manufacturing facilities, but not here.. Here we work in a "Single Order" flow and it doesn't matter in the shop and nothing is manufactured for inventory, the only chance there is or can be a confusion is in our programming and or work order/routers etc..
Each Bed Style has five different sizes and we know there are "Same" interchangeable components such as the Headboard and Footboard posts, however, every post is a different part number, makes my end super easy not having to worry about the parts being exactly the same. Those "Posts" only get used for that "Style" which is also a factor. Plus we don't sell "Replacement" parts either. So what David Matula mentioned works for us, but not the next guy..
Hi Keith Panik
You are certainly in good hands in this discussion (with John, Frederick, Matt, Scott, Jim and David). I’ll look at your model later this afternoon and see if I can add anything. I would reiterate what others have suggested - that creating a top down assembly is best managed with a SSP that drives the basic form of every part below it in the Feature Manager. Cross referencing between parts is a recipe for disaster (as we all have experienced). The SSP may contain sketch elements – but in addition to what has been mentioned - and to make it easier to visualize - it may also contain a solid model of the basic form and features of your assembly. There are advantages to either approach.
More soon, CSS
Great for you to jump in here Chris Scarlett - always appreciate your input. My next project will be using Part in Part and I want to experiment with Blocks as well. I think using blocks in the SSP in some instances would be a huge plus...
OK, thanks for all the information. I am retrying this with my master sketch in the assembly. I can insert new parts and convert the Master Sketch lines to the new part for extruding. All good. I am now struggling to figure out how to give these new parts a part name and file name. The help says I should get a save as dialog upon insertion but I am not seeing that. Do I just rename them once inserted?
I'm not quite there yet but I am wondering how I get to each individual part for each separate configuration? Will the configurations be added to each part?
TIA
Keith Panik wrote:
I'm not quite there yet but I am wondering how I get to each individual part for each separate configuration? Will the configurations be added to each part?
TIA
Hi Keith
Yes - This is a useful page from the help that explains it better than I could
2018 SOLIDWORKS Help - Best Practice for Configurations with External References
OK so I've re-modeled the assembly with my master sketch driving the parts from the assembly. Everything updates perfectly in that assembly (each and every time). Next step I put that sub-assembly into the next assembly. Add configurations, call out the different configurations in my sub-assembly and they don't update until I "edit component", then it updates.
This is a pretty typical workflow I've used for years, Is this even doable in solidworks?
Keith,
I am far from an expert at top down, for that you need to talk to John Stoltzfus or Matt Peneguy. But I think you want your driving sketch to be in the top level. You could place a 3D sketch first in your model tree, I think you may need to create a new assembly and do the sketch first thing.
John and Matt have several posts talking about top down. You should search for "SSP" on the forum.