SOLIDWORKS Design & Help

Parts can be locked by enabling the locking freeze bar for the feature tree, but that locks everything. SW help has some more info.

If you made the configurations with a design table, you could try locking or protecting the cells. But a determined user could still modify values outside of the table.

I want to lock my ASM ,to go to the next configuration and when I change something in to the next configuration not to affect the mates.I don't want the mates to have relations to the previous configurations so whatever change I make in mates to be considered only to the specific configuration that I am changing.

If someone can give me an Idea how to do that I will be very thankful

It really depends on what kind of mates you are using, for example: if you are using distance mates, you could just create a design table or configure the distance mates, any changes that you make to one configuration shouldn't affect other configurations.

If you are using other mates (like coincident, concentric, tangent, etc), you could configure the mate state (suppress/unsuppress), and create mates for each configuration, for example: you would have "Mate1" unsuppressed for configuration "1" and suppressed for all other configurations, then "Mate2" unsuppressed for configuration "2" and suppressed for all other configurations, and so on.

Hope this helps.

When you create a new configuration, the properties bar has a section called "Advanced Options". You can select "Suppress new features and mates" and "Suppress new components".

This means that anything added in another configuration will not show up in this configuration. These can be configuration specific, so you can turn them on for one configuration and off in another.

Take note, if you delete something it will be gone. You need to use suppress if you want to remove a part.

Hello, everyone.

Hope you all are having a very good night/day.

Sorry for asking this as a reply, but seems to me like is some sort of the same question i have.

I'm looking for some advice/help as I have no more ideas of what's happening in my assembly.

Here is the thing: I have a main door assembly with 2 subssemblies in it:

01. Frame (Jamb)

02. Door Itself.

This main assembly have multiple configurations for sizing purposes. Important to say is that the parts inside those 2 subassemblies have configurations for sizes as well, looking something like this:

1. Unit (configurations)

1.1 Jamb (configurations)

1.1.1 Jamb parts (configurations)

1.2 Door (configurations)

1.2.1 Door parts(configurations)

By themselves, Frame and Door, behave as they are supposed to be working, but when they are together on the main assembly, everything goes nuts. Anytime I open it, seems like mates within both sub assemblies are suppressing or something like that.

I can provide a video of this if needed.

If you supress and unsupress mates without checking for which configuration they are applying to, you will allways have a problem.You have to create a group of mates then you have to configure them for all configurations .If you have new components in some configurations or parts that are not been used in other configurations you have to be verry carefull.Before to suppress features and parts.Click right button on them,clik configurations and chek them in which configurations to be used by chekbox.

It took me 3 months to find out 'why me Oh god' is this happening to me!

Use only coordinate systems for mates and coincident and distance only.The tangent mate is not a good choice of mate try to avoid it.When you mate everything according to the coodinate system and configure everything,Create yourself a designe table so you can control every dimention that you have to change.