CAD Forum

In Creo, I can add a component to an assembly, and then control its size using rules (it's called "flexible components"). How is that done in Solidworks?

I have a pin that is cut to length and put into the product. I don't want to put an eight-foot rod into the assembly and use an assembly cut to cut it down to six inches.

Configure the dimension?

KSHansen

You can also add an in-context relation by editing the part in the assembly, such as setting an extrude feature to end at the surface of some other part. Note that we never use in-context relations, as it screws us over in file management. You could also drive everything with a layout, though we don't do that either.


"I don't want to put an eight-foot rod into the assembly and use an assembly cut to cut it down to six inches."

In the case you describe, we wouldn't either, but if our actual assembly involved doing something like that, cutting something to size in the process of creating the assembly, then that is how we would model it.

Dwight

I'd also recommend using configurations.

Careful with configurations, having the rod's length changed will also affect the rod's length displayed in your BOM.

As Dwight said, if I wanted to take something of a given length and have it cut down, I'd most likely have a sub-assembly created to do the assembly cut on it. Makes the displaying of the process easier too.

mattpeneguy wrote: ↑Tue Jun 28, 2022 1:04 pm Configure the dimension?

Configure Dimension does not come up when I right-click the dimension.

I'm not quite sure how this works, but I'm also trying to avoid having to create a huge list of configurations in the pin model, to go along with the huge list of configurations in my assembly. Fortunately the pin model is a generic model - not a model that is used on a production drawing - so I could do odd things to it, if need be. But the model is just for visuals, not for production records.

KSHansen wrote: ↑Tue Jun 28, 2022 12:10 pm I don't want to put an eight-foot rod into the assembly and use an assembly cut to cut it down to six inches.

KSHansen wrote: ↑Tue Jun 28, 2022 2:13 pm I'm also trying to avoid having to create a huge list of configurations in the pin model, to go along with the huge list of configurations in my assembly.

Those seem like the 2 most straightforward options to me. If neither of those work, I'm not sure what to recommend.

Dwight wrote: ↑Tue Jun 28, 2022 1:39 pm KSHansen

You can also add an in-context relation by editing the part in the assembly, such as setting an extrude feature to end at the surface of some other part. Note that we never use in-context relations, as it screws us over in file management. You could also drive everything with a layout, though we don't do that either.

"I don't want to put an eight-foot rod into the assembly and use an assembly cut to cut it down to six inches."

In the case you describe, we wouldn't either, but if our actual assembly involved doing something like that, cutting something to size in the process of creating the assembly, then that is how we would model it.

Dwight

I've never worked with changing component dimensions in an assembly, except for the aforementioned flexible components. So what you're saying sounds like it might work for me, but I don't really understand it. Like, "drive everything with a layout." Not sure what that means.

By the way, Dwight, you look familiar. Did you ever play The Affable Neighbor in a TV sitcom?

KSHansen wrote: ↑Tue Jun 28, 2022 2:13 pm Configure Dimension does not come up when I right-click the dimension.

I'm not quite sure how this works, but I'm also trying to avoid having to create a huge list of configurations in the pin model, to go along with the huge list of configurations in my assembly. Fortunately the pin model is a generic model - not a model that is used on a production drawing - so I could do odd things to it, if need be. But the model is just for visuals, not for production records.

I have a hunch you're looking for driving a part length ad hoc. This is where you model the pin at 3", but want it to be 5" in one assembly and 6" in another without actually changing the part model. Solid Edge has a similar feature but they call it Adjustable Part.
No, SWX has nothing of the sort, but I guess SE doesn't have easy configurations either.....

mike miller wrote: ↑Tue Jun 28, 2022 2:34 pm ... This is where you model the pin at 3", but want it to be 5" in one assembly and 6" in another without actually changing the part model. ...

Correct

On the other hand, since the pin model isn't used for anything else, I could have its length updated every time I open a new configuration of the assembly...

mike miller wrote: ↑Tue Jun 28, 2022 2:34 pm I have a hunch you're looking for driving a part length ad hoc. This is where you model the pin at 3", but want it to be 5" in one assembly and 6" in another without actually changing the part model. Solid Edge has a similar feature but they call it Adjustable Part.

image.png

No, SWX has nothing of the sort, but I guess SE doesn't have easy configurations either.....

Nice option in SE that I wish SWX had.

SolidWorks has what's called a "Flexible Part". You build the rod length "in context". Then insert it into other assemblies and toggle it "Flexible" which prompts to select an assembly reference to control it length.

KSHansen wrote: ↑Tue Jun 28, 2022 12:10 pm In Creo, I can add a component to an assembly, and then control its size using rules (it's called "flexible components"). How is that done in Solidworks?

I have a pin that is cut to length and put into the product. I don't want to put an eight-foot rod into the assembly and use an assembly cut to cut it down to six inches.

Make those components flexible.

https://help.solidworks.com/2022/englis ... onents.htm

Alin wrote: ↑Tue Jun 28, 2022 6:40 pm Make those components flexible.

https://help.solidworks.com/2022/englis ... onents.htm

The part I don't like is having to build it in-context. I suppose I don't have to keep that assembly, but still feels like a kludged together function. I should be able to establish the "flexible" geometry parameters in the part directly.

jcapriotti wrote: ↑Tue Jun 28, 2022 10:54 pm The part I don't like is having to build it in-context. I suppose I don't have to keep that assembly, but still feels like a kludged together function. I should be able to establish the "flexible" geometry parameters in the part directly.

Jason

How would you prefer to establish those parameters in the part? Like creating a look-up table in the part?

Dwight

KSHansen wrote: ↑Tue Jun 28, 2022 2:13 pm Configure Dimension does not come up when I right-click the dimension.

I'm not quite sure how this works, but I'm also trying to avoid having to create a huge list of configurations in the pin model, to go along with the huge list of configurations in my assembly. Fortunately the pin model is a generic model - not a model that is used on a production drawing - so I could do odd things to it, if need be. But the model is just for visuals, not for production records.

From a post further down I'm guessing you tried this in the Assembly. If the dimension belongs to the Part you need to configure it in the Part, then reference the desired Part configuration in the Assembly.

I know I said yesterday that configurations were the way to go, but if this is a library part that will be used extensively, in multiple projects, then configurations might not be the best choice. The simplest solution may be to just copy and paste the Part, give it a new name, and edit the length dimension to what you need for the current project. If it's used multiple times in the same Assembly, then I would use configurations.

Dwight wrote: ↑Wed Jun 29, 2022 7:08 am Jason

How would you prefer to establish those parameters in the part? Like creating a look-up table in the part?

Dwight

Great question there Dwight. I'd love to see something as people explain in SolidWorks, but I have a hard time figuring out how it would work.

KSHansen wrote: ↑Tue Jun 28, 2022 2:13 pm Configure Dimension does not come up when I right-click the dimension.

I'm not quite sure how this works, but I'm also trying to avoid having to create a huge list of configurations in the pin model, to go along with the huge list of configurations in my assembly. Fortunately the pin model is a generic model - not a model that is used on a production drawing - so I could do odd things to it, if need be. But the model is just for visuals, not for production records.

Just to clarify on this @KSHansen, you have to open the part to have access to "Configure Dimension". That, or you can "Edit Part" in the assembly to configure the dimension. I think it's this way so that you don't inadvertently select it when you think you may be editing an assembly level dimension.
Unfortunately the software doesn't always work the way we think that it should. But, you can usually do what you need and I think people have given you a lot of options. Maybe give a few a chance and then let us know what works for you?

You can design the part in the context of the assembly, with all of the references being to other parts in the assembly. What is added by making the component flexible?

SPerman wrote: ↑Wed Jun 29, 2022 9:37 am You can design the part in the context of the assembly, with all of the references being to other parts in the assembly. What is added by making the component flexible?

When you add the part to another assembly, the in-context reference is not solved since the original assembly is not open. You can toggle the part as flexible and it will prompt for a new external references which will drive the instance geometry. You can even insert a second instance and drive it with a different external reference in the same assembly.

That makes sense. Thanks for the information. That is a very powerful tool.

Dwight wrote: ↑Wed Jun 29, 2022 7:08 am Jason

How would you prefer to establish those parameters in the part? Like creating a look-up table in the part?

Dwight

A wizard interface like smart components that asks you to pick the features to drive. And stores them in a node in the tree for later editing.

So say I pick an extrude feature, it should show the end condition which I should be able to set "Up to (Flexible)"

Here's an example of a rod.....no configuration. The Length is controlled by a plane with an Up to surface condition.

Insert into assembly and toggle flexible, select the new assembly plane. Works with pattern instances as well.

jcapriotti wrote: ↑Tue Jun 28, 2022 3:38 pm SolidWorks has what's called a "Flexible Part". You build the rod length "in context". Then insert it into other assemblies and toggle it "Flexible" which prompts to select an assembly reference to control it length.

This worked! I struggled with it for a while, before I got it to work, and I'm still not entirely sure what I did. Also, when I opened a different configuration of the assembly, the planes used to define the length were suppressed, so I had to unsuppress them in each config. Strange. Anyway...

Now the pin changes length with the size of the assembly, and I don't have to deal with setting up configurations in the pin model. The only downside to be aware of is that every time I open the pin model, its length matches whatever it was last, in the assembly. That's not a problem in this case, because I'm not using a model of a production part - I set it up specially for this situation.

Thanks, J!

KSHansen wrote: ↑Thu Jun 30, 2022 2:20 pm This worked! I struggled with it for a while, before I got it to work, and I'm still not entirely sure what I did. Also, when I opened a different configuration of the assembly, the planes used to define the length were suppressed, so I had to unsuppress them in each config. Strange. Anyway...

Now the pin changes length with the size of the assembly, and I don't have to deal with setting up configurations in the pin model. The only downside to be aware of is that every time I open the pin model, its length matches whatever it was last, in the assembly. That's not a problem in this case, because I'm not using a model of a production part - I set it up specially for this situation.

Thanks, J!

Going to the configuration properties before adding the planes and de-selecting this option would have fixed that. (I know it's too late, but it might help next time.)

Glenn Schroeder wrote: ↑Thu Jun 30, 2022 2:32 pm Going to the configuration properties before adding the planes and de-selecting this option would have fixed that. (I know it's too late, but it might help next time.)

Yeah, that looks like it. Um... where do I find that? I did a search for configuration properties in Solidworks, and nothing come ups.

Click on the configurations tab, and then right click on a given configuration.

SPerman wrote: ↑Thu Jun 30, 2022 4:38 pm Click on the configurations tab, and then right click on a given configuration.

Ah! It was hidden under an "Advanced" button. Thank you!

Is the pin a purchased part?
Do you need a drawing to show the cut length of the pin?
If it's a pin you buy in 8ft. lengths, I'd make a weldment profile of the pin, and put the description and part number in the profile.
Then use weldments and make it whatever length you need.

Or,
Draw the pin at the 8ft. length, and create a cut.
Create configurations for different cut lengths, and configure the cut dimension.
Then you just reference that particular configuration of the part in the assembly.

20 years of CAD experience, and I've always had assembly-based, or in-context definitions of parts bite me at some point...

IndianaDave wrote: ↑Thu Jul 07, 2022 11:10 am Is the pin a purchased part?
Do you need a drawing to show the cut length of the pin?
If it's a pin you buy in 8ft. lengths, I'd make a weldment profile of the pin, and put the description and part number in the profile.
Then use weldments and make it whatever length you need.

Or,
Draw the pin at the 8ft. length, and create a cut.
Create configurations for different cut lengths, and configure the cut dimension.
Then you just reference that particular configuration of the part in the assembly.

20 years of CAD experience, and I've always had assembly-based, or in-context definitions of parts bite me at some point...

The pin model is not for a production drawing. It's just for visuals, to make pictures of the assemblies to use for whatever purposes we need them for.

For this model, I ended up with 50 configurations, and more are possible. That's a lot of configurations to create in the pin, and then set in the assemblies, and chance for error. I would use this same pin in other models, with a similar number of possible lengths, but given the requirement for in-context, I'm not sure this is possible. Anyway, even with the time I spent trying to figure out how to make this work, I think I saved myself a lot of time.

You have been presented several good options but before I answer I'd like to have answer first.

How is the part managed and recorded in your CAD BOM, manufacturing BOM or shop floor? This answer should really drive how you manage your part in the other systems.

The part is not managed in a BOM. It doesn't go to the shop floor since this is just for making pretty pictures for literature. The pin model isn't even connected to a real-world part.

I don't want to create hundreds of configurations for the pin, or create a new config for the pin every time I create a new config for the assembly, I just want to put the pin into the assembly and not have to think about it again.

KSHansen wrote: ↑Wed Aug 03, 2022 10:30 am I don't want to create hundreds of configurations for the pin, or create a new config for the pin every time I create a new config for the assembly, I just want to put the pin into the assembly and not have to think about it again.

Not sure if it was mentioned, but making it "virtual" is another option, then you can edit the copy inside the assembly. Same as copying the file over and over, you just have to store the file if its virtual.