CAD Forum

I've read through the Barrataria and the Skeleton Sketch Part (SSP) Presentation PDFs, and I've been experimenting with using SSPs in my furniture models for the last few months. Somewhere (Youtube video?) I learned to insert a SSP into a each part in an assembly which seems to work pretty well, but the Barrataria PDF talks about inserting the SSP as the first part in an assembly instead of the individual parts. Which method is correct?

The one "problem" I have with inserting the SSPs into each part of the assembly is that when I first open the assembly, there is a ? next to each part in the assembly, and if I drill down to inside the parts the ? comes from the SSP. If I open the part, then edit the SSP (but don't change anything) and save and close, the ? goes away for all of the parts in the assembly. I don't understand why this happens, but it doesn't appear to affect anything. What is causing the ?

Thanks,

Jim

Jim

The SSP file does not have to be in the assembly if it's in the component part files. I find it it best to not create in-context relations, meaning relations made within the assembly, which can easily lead to trouble. Leaving the SSP out of the assembly helps you to avoid those problems.

On the other hand, if the SSP file is a component of the assembly, then it automatically opens the SSP when you open the assembly, and Solidworks will not report a missing external reference with a ? You can also do that instead by opening the SSP manually. You shouldn't have to edit anything.

The ? means that the external reference is not open. Select the menu items File / Find References to show a list of References. Any that are not open will be marked "Not Open".

When opening an assembly with external references, you should get the option to open all the referenced documents. If you don't see this, you might want to go to your system options and uncheck it under Messages/Errors/Warnings
Dwight

@JimLancaster To add to what to Dwight said, check this setting in options. For SSP, you want it to open all referenced parts. The description is bad as it only applies to part to part references. Assembly reference are always loaded.

Dwight wrote: ↑Fri Dec 31, 2021 10:35 am The SSP file does not have to be in the assembly if it's in the component part files. I find it it best to not create in-context relations, meaning relations made within the assembly, which can easily lead to trouble. Leaving the SSP out of the assembly helps you to avoid those problems.

To be clear, do you recommend inserting the SSP part into the component part's of an assembly?

I've been trying to recreate one of my models using the guidelines provided in @mattpeneguy's Barataria.PDF and, but there is enough ambiguity in it to make it a little challenging for a relatively new Solidworks user like me to follow. Matt's PDF clearly talks about making the SSP part the first part in an assembly (and not inserting the SSP part into the individual parts of the assembly). I'm guessing there must be a reason.

My woodworking/furniture models are quite modest in size, having no more than a few dozen parts. But I've built each model to be very flexible, with different configurations defining a dozen or more sizes. And a chest of drawers could have any number of drawers of different sizes. Using SSPs has been key to that along with figuring out how to gracefully blend in Equations and Design Tables. I'm just trying to make sure that I'm following a well trodden path and not blazing a trail on my own.

Jim

I haven't modeled much furniture, but I've built some, and I often model Parts with multiple bodies. I'm not at all sure that an Assembly would be a better option than a multiple body Part for furniture.

Dwight wrote: ↑Fri Dec 31, 2021 10:35 am Jim

The SSP file does not have to be in the assembly if it's in the component part files. I find it it best to not create in-context relations, meaning relations made within the assembly, which can easily lead to trouble. Leaving the SSP out of the assembly helps you to avoid those problems.

On the other hand, if the SSP file is a component of the assembly, then it automatically opens the SSP when you open the assembly, and Solidworks will not report a missing external reference with a ? You can also do that instead by opening the SSP manually. You shouldn't have to edit anything.

The ? means that the external reference is not open. Select the menu items File / Find References to show a list of References. Any that are not open will be marked "Not Open".

When opening an assembly with external references, you should get the option to open all the referenced documents. If you don't see this, you might want to go to your system options and uncheck it under Messages/Errors/Warnings

image.png

Dwight

This is what I do.

I add the MasterModel as the first part of a component (part). Then I also add the MasterModel as a component in the assembly. It is a component in the assembly as an envelope part, not for linking to inside the assembly (as that is already being done via the part file), but so that the MasterModel is opened when the assembly is opened, and for potential mating.

@dpihlaja That's the way I've been doing it for a few months, but I was having weird issues as I switched between different configurations. Features would break. Dimensions defined by Design Tables would revert to being hard defined within a sketch. It didn't happen all the time, but often enough to make me think I didn't completely grok the concept of a Skeleton Sketch Part. That's what led me here to learn more.

I just finished recreating a 7 drawer chest with the SSPs the first part in the case & drawer assemblies as I think is described in the PDFs provide by @mattpeneguy and @Roasted By John. It seems to be holding up well to changes in random dimensions. One thing I have noticed is that it was more difficult (impossible?) to create mechanical mates for my french cleat drawer slides using this method. (I'd be happy to share the model with anyone who'd like to review it.)

I will repeat the exercise with the SSPs inserted into the individual parts and see if I get a repeat of the (seemingly) random errors I was getting before and perhaps uncover some differences between using the two methods.

Jim

I know John recommended the sketch live in the assembly, and the parts make the references at the assembly level. I believe that was due to problems like what you are describing, but I can't say for sure. I've always done it that way and it has been rock solid for me.

I had played with SSP recently too and my preference is to insert the SSP into each part (or whichever part that need the SSP)

Some of my rationale is that:
1. This make collaborating with other more easily as everyone just Pull the SSP into their part as needed (better to have someone break their own part than breaking everyone's part eh?)
2. The part can be place in different assembly level more easily (eg: Part A and B at level 1 whereas Part C at level 2)
3. My personal practice is to avoid in-context reference at much as possible
4. (I never really did this but....) Inserting the SSP into each part make it easier to break the reference when needed

I do not use much configuration with SSP nor design table so i cant comment on that
As for mechanical mate, i dont think i have any issue with my current approach

My 2cents is that use whatever that fit your need.

JimLancaster wrote: ↑Mon Jan 03, 2022 5:22 pm @dpihlaja That's the way I've been doing it for a few months, but I was having weird issues as I switched between different configurations. Features would break. Dimensions defined by Design Tables would revert to being hard defined within a sketch. It didn't happen all the time, but often enough to make me think I didn't completely grok the concept of a Skeleton Sketch Part. That's what led me here to learn more.

I just finished recreating a 7 drawer chest with the SSPs the first part in the case & drawer assemblies as I think is described in the PDFs provide by @mattpeneguy and @Roasted By John. It seems to be holding up well to changes in random dimensions. One thing I have noticed is that it was more difficult (impossible?) to create mechanical mates for my french cleat drawer slides using this method. (I'd be happy to share the model with anyone who'd like to review it.)

I will repeat the exercise with the SSPs inserted into the individual parts and see if I get a repeat of the (seemingly) random errors I was getting before and perhaps uncover some differences between using the two methods.

Jim

Once you fully grok SSP let me know, because I still haven't...It's a constant learning process. Some things work great and some things break easily. I wish there was a manual, but I guess we all have to write our own.

SPerman wrote: ↑Mon Jan 03, 2022 5:49 pm I know John recommended the sketch live in the assembly, and the parts make the references at the assembly level. I believe that was due to problems like what you are describing, but I can't say for sure. I've always done it that way and it has been rock solid for me.

I read that and just so no one is confused, there were no assembly level sketches involved in what John used. I think that's one of the reasons he liked the name Skeleton Sketch Part. It's part to part references only. You put the sketch part at the top of the feature tree and all of the parts below it reference it. If you have subassemblies, then you put a separate sketch part below the top level sketch part and then put that sketch part in the subassembly. Then the top level sketch part can have references to parts or sketch parts going DOWN the feature tree only, never up.
Hopefully the below makes it clear:

0.SSP
1.SSPA
1.SSPB
SUBASMA
1.SSPA
1.PartA1
1.PartA2
SUBASMB
1.SSPB
1.PartB1
1.PartB2
0.Part1
0.Part2

0.SSP drives 1.SSPA, 1.SSPB, 0.Part1, and 0.Part2. 1.SSPA drives 1.PartA1 and 1.PartA2. 1.SSPB drives 1.PartB1 and 1.PartB2.
You can add more depth but you can only drive relations one level.

I see no need to have a skeleton sketch in a separate part. The master sketch can reside at the top level assembly, and then copied in-context down through the assembly tree. This has always worked well for me.

JimLancaster wrote: ↑Mon Jan 03, 2022 5:22 pm @dpihlaja That's the way I've been doing it for a few months, but I was having weird issues as I switched between different configurations. Features would break. Dimensions defined by Design Tables would revert to being hard defined within a sketch. It didn't happen all the time, but often enough to make me think I didn't completely grok the concept of a Skeleton Sketch Part. That's what led me here to learn more.

I just finished recreating a 7 drawer chest with the SSPs the first part in the case & drawer assemblies as I think is described in the PDFs provide by @mattpeneguy and @Roasted By John. It seems to be holding up well to changes in random dimensions. One thing I have noticed is that it was more difficult (impossible?) to create mechanical mates for my french cleat drawer slides using this method. (I'd be happy to share the model with anyone who'd like to review it.)

I will repeat the exercise with the SSPs inserted into the individual parts and see if I get a repeat of the (seemingly) random errors I was getting before and perhaps uncover some differences between using the two methods.

Jim

I have moved away from a whole Skeleton Sketch mentality and started using a multibody part as my master model. It pulls into other parts easier, and gives me good geometry that is easy to change and then I just need to delete the extra bodies and use the body that I want for that part.

HerrTick wrote: ↑Tue Jan 04, 2022 10:27 am I see no need to have a skeleton sketch in a separate part. The master sketch can reside at the top level assembly, and then copied in-context down through the assembly tree. This has always worked well for me.

Not trying to contradict you, just wanted to add that in my experience assembly sketches work reasonably well for small to medium assemblies. Having the reference sketches and other reference entities residing in a part allow for more freedom in achieving one-step dependencies between files.

mattpeneguy wrote: ↑Tue Jan 04, 2022 8:31 am Once you fully grok SSP let me know, because I still haven't...It's a constant learning process. Some things work great and some things break easily. I wish there was a manual, but I guess we all have to write our own.

I don't know whether to be amused, relieved, or alarmed by this!

dpihlaja wrote: ↑Tue Jan 04, 2022 11:01 am I have moved away from a whole Skeleton Sketch mentality and started using a multibody part as my master model. It pulls into other parts easier, and gives me good geometry that is easy to change and then I just need to delete the extra bodies and use the body that I want for that part.

I am kind of the opposite I guess..
I originally use multibody part as most of my master model (especially if it involve some sort of mechanism), but the performance start slowing down when thing get more and more complex.

So, in the end, i still use multibody for my rough concept, but start to transition to SSP once i have some basic layout/idea of the concept

At the risk of bombing this thread with way too much detail, here are the results of my experiment:

My Seven Drawer Chest has one Case Assembly which contains the Case parts (side, back, top & bottom) and 7 instances of a Drawer Assembly. The drawers are of 3 different sizes which are controlled using Design Table configs. The drawers hang on french cleats. The top cleat attaches to the side of drawer, and the bottom cleat which the drawer hangs on attaches to the inside of the case.
In recreating the chest, I ran into an issue using derived sketches as recommended in the Barataria PDF. Both the top and bottom cleats are derived from the same two sketches in the Drawer SSP. The top cleat is obviously a part of the Drawer Assembly, but what about the bottom cleat? Is it more correctly a part of the Case Assembly?

In my first pass, I created one Cleat part that contained a "top" and "bottom" config. I attached a "Cleat (Top)" to drawer side in the Drawer Assembly and inserted the first instance of the Drawer Assembly into the Case Assembly. Then I inserted a "Cleat (bottom)" into the Case Assembly, but I guess because the Cleat part was created with an InPlace mate, I couldn't add additional mates to position it correctly in the Case. It appeared that the bottom cleat had to be a part of the Drawer Assembly too.

0 - Case Assembly
0 - Case SSP
0 - Case Side
0 - Case Top
0 - Case Back
1 - Cleat (bottom) [derived sketch, inplace mate]
1 - Drawer Assembly (size1,size2,size3)
1 - Drawer SSP (size1,size2,size3)
1 - Drawer Face (size1,size2,size3)
1 - Drawer Side (size1,size2,size3)
1 - Drawer Back (size1,size2,size3)
1 - Drawer Bottom (default)
1 - Cleat (top) [derived sketch, inplace mate]

In my second pass, I separated the top & bottom cleats into two distinct parts and put both in the Drawer Assembly. Then I inserted seven Drawer Assembly instances of 3 different sizes into the case. Everything looked pretty good until I hid the Case Side to look at the cleats and found the cleats weren't in the right places. They looked to be randomly attached to the sides of the Drawer boxes. When I edited a Drawer Assembly to take a closer look, the cleats for that Drawer Assembly (and the others of the same size/config) moved to the correct position, but all of the other cleats moved too--to the wrong place for their drawer sizes. I played around with it for a while, but I could not figure out why that was happening.

0 - Case Assembly
0 - Case SSP
0 - Case Side
0 - Case Top
0 - Case Back
1 - Drawer Assembly (size1,size2,size3)
1 - Drawer SSP (size1,size2,size3)
1 - Drawer Face (size1,size2,size3)
1 - Drawer Side (size1,size2,size3)
1 - Drawer Back (size1,size2,size3)
1 - Drawer Bottom (default)
1 - Top Cleat (default) [derived sketch, inplace mate]
1 - Bottom Cleat (default) [derived sketch, inplace mate]

In my third and final pass, I decided to take a completely different approach. I removed the cleats from the Drawer Assembly and recreated a single Drawer Cleat part from scratch, but this time I inserted the Drawer SSP part into it, then added the top/bottom configs. I inserted the "Drawer Cleat (top)" into the Drawer Assembly then rebuilt the Case Assembly to update the seven Drawer Assembly instances in it. The top cleats now appeared in the correct position for all drawers. Next I inserted 7 instances of "Drawer Cleat (bottom) into the Case Assembly, and manually each into position, mating each to the bottom of a top cleat of a drawer and to the Case Side. Now everything appears to be working as it should.

0 - Case Assembly
0 - Case SSP
0 - Case Side
0 - Case Top
0 - Case Back
1 - Cleat (bottom) [inserted Drawer SSP, manual mate]
1 - Drawer Assembly (size1,size2,size3)
1 - Drawer SSP (size1,size2,size3)
1 - Drawer Face (size1,size2,size3)
1 - Drawer Side (size1,size2,size3)
1 - Drawer Back (size1,size2,size3)
1 - Drawer Bottom (default)
1 - Cleat (top) [inserted Drawer SSP, manual mate]

In conclusion, I employed a more "hybrid" approach to using the SSP. The Case and Drawer assemblies both have SSPs that are stand alone parts within their respective assemblies, but the Drawer Cleat has the Drawer SSP part inserted into it. The model now appears to be working as expected, but I will continue to play around with it and see where it breaks.

Thanks for the feedback,

Jim

Can you upload your asm or some dimensions? What are the variables? Is it always going to have 7 drawers?

The problem you have is reusing drawers. Since you have 3 different size drawers, then the overall height has to be based on the drawer sizes...Not insurmountable, but requires careful planning.

I remember seeing something like this done in DriveworksXpress. I found something simpler, but it may be worth watching to see if it's something that could help. Though the complexity seems it might require purchasing Driveworks Solo. Here's Xpress:


Here's something similar to what you are doing with Solo:

mattpeneguy wrote: ↑Wed Jan 05, 2022 3:39 pm Can you upload your asm or some dimensions? What are the variables? Is it always going to have 7 drawers?

I would be happy to upload my files, but just uploading the images in my previous post nearly caused me to tear my hair out. I tried to attach an .EASM file, but apparently that's not allowed. I've attached a ZIP file containing a pack and go of the whole model to this reply. Let's see if that works. If it doesn't, I'll gladly email them or post them somewhere where they can be downloaded for those who are interested.

Literally everything in the model is tied to a variable in either the Equations or a Design Table. The dimensions of the case can be adjusted, the material thickness, even the number of box joint tabs where the edges of the Case parts meet. In its current form, there are two Case configs ( Type1=6 drawers, Type2=7 drawers), but adding another (e.g., Type3 with 5 drawers) should be rather straightforward. The drawer dimensions are similarly flexible. I'd be happy to share the how/why I chose to model the chest in this way. The short answer is that I wanted a flexible model that could be cut on my CNC, but there is a lot more to it than that if anyone is interested. I'm trying to be kind to those skimming this thread by limiting the length of my already wordy posts.

Note that the nomenclature in the model is slightly different than what I described in my previous post. My ultimate goal is to build casework (chest of drawers, credenzas, etc) using my CNC, but to start with I designed and built a "Shopcart" that sits on 3" casters in my shop. So as you look into the model Case = Shopcart and Cleat = Runner.

Finally, a disclaimer: I'm completely self-taught. I was a long-time Sketchup user (which is much more common in woodworking circles), but I retired just before the start of the pandemic and my mechanical engineer sons convinced me to switch to Solidworks now that I had the time learn it. One taught me the basics, and I took it from there. I have no idea what bad habits I've accumulated or what you experienced engineers/cad techs will think when you see this model. Please be kind.

Jim

Sorry...We're on Windows 7 and I can't upgrade past 2020. So I can't open your 2021 assembly. I wonder if @Rob is around. He's done some very complicated assemblies with equations. And he's done a lot of cool woodworking projects too.

I haven't read the whole story sorry but yep I'm a woodworker.

I've tried about every way I can think of but am of the conclusion that any serious solution requires api support.

What I've often done is to create a skeleton part or parts and have them as an envelope in every relevant assembly.
I tend to not make external references to the SSP in the assembly context unless I have to or I am manipulating the equations in the assembly itself. The skeleton is mostly there as scaffolding for mates.
The parts themselves have the skeleton injected into them as part in part, but I generally will not include any geometry, just the model dimensions.

Let me show an example.
Here's my skeleton. I am using only planar surfaces and have my top level equations. This is the bones and the brain! Here's one of the sub assemblies
and the principal sub
As you can see below my skeleton is in every sub In this particular project because of the sheer number of configurations I had to remove the inserted part external reference and automate the updating of dimensions from a higher level survey skeleton It ended up being a monster Having a skeleton is generally a very useful thing and there are many ways to use it.

I like to think of it as a single place to keep your important shared faces/dimensions/planes/axes/etc...

Use it however you want

Ultimately it depends on the performance you want to achieve how far you should go.

In my latest project I have foregone an ssp entirely and have instead created my part configurations so that parts that share the same length are the same. That's a real fun way of working as you can make edits from up the assembly tree. It has the benefit of not adding external refs, but has it's limitations. I like it for prototyping and one-offs

Rob wrote: ↑Thu Jan 06, 2022 5:15 am I haven't read the whole story sorry but yep I'm a woodworker.

I've tried about every way I can think of but am of the conclusion that any serious solution requires api support.

What I've often done is to create a skeleton part or parts and have them as an envelope in every relevant assembly.
I tend to not make external references to the SSP in the assembly context unless I have to or I am manipulating the equations in the assembly itself. The skeleton is mostly there as scaffolding for mates.
The parts themselves have the skeleton injected into them as part in part, but I generally will not include any geometry, just the model dimensions.

Let me show an example.
Here's my skeleton. I am using only planar surfaces and have my top level equations. This is the bones and the brain!
image.png

Here's one of the sub assemblies

image.png

and the principal sub

image.png

As you can see below my skeleton is in every sub
image.png

In this particular project because of the sheer number of configurations I had to remove the inserted part external reference and automate the updating of dimensions from a higher level survey skeleton
image.png

It ended up being a monster
image.png

Having a skeleton is generally a very useful thing and there are many ways to use it.

I like to think of it as a single place to keep your important shared faces/dimensions/planes/axes/etc...

Use it however you want

Ultimately it depends on the performance you want to achieve how far you should go.

In my latest project I have foregone an ssp entirely and have instead created my part configurations so that parts that share the same length are the same.
image.png
image.png
That's a real fun way of working as you can make edits from up the assembly tree. It has the benefit of not adding external refs, but has it's limitations. I like it for prototyping and one-offs

Well I was right...Once again proving that I'm playing checkers, while @Rob is playing 3-D chess...