I was wondering if there is any way to automatically fully define an assembly? I have a number of fasteners than have concentric mates but are still allowed to spin freely and I would like to fully define them all.
Good morning Jeff,
Your parts should have mate references such as cylindrical edges than you can reduce the steps to mate, if you use the pin in hole mate, available in the drag and drop mode.
The other thing you may want to look into is the multi selection feature that is available in the mate pop up menu, see attached, you can also check which mates you would like to have placed in a folder. What I do in with fasteners, I select an edge of an assembly part and then go parallel and select faces or planes on each item and I'm done.
This may not possible in one go, but You can simply use LOCK mate to lock all .
Welcome to the Forum. There have been several discussions here on the subject of fully defining hardware and there seems to be a consensus that SW will be faster without that extra mate to solve, so I just leave mine free to rotate. With that being said, I am not aware of any way to lock them all short of an extra mate with each individual part. You can use the lock mate as Ajay suggested, but I would probably just use a parallel mate with one of the planes of the fastener and another plane in the assembly.
Thanks! That was my plan (mating a plane to be parallel) but even with a small assembly there may be 32 induvidual fasteners. Maybe I will put all the fasteners in a folder so the (undefined symbol) doesn't always have me wondering whether the part is a fastener or not!
Welcome to the forum.
If these fasteners were done using patterning then these are the results you will see.
Ajay and Glenn are correct in what they told you.
I know what you mean, that bugs me too. I wish the folks at SW would fix it so there was a different symbol for Toolbox parts that can only rotate.
The problem with either patterning or perhaps having a solution for toolbox parts are that this is not always the case; patterning doesnt always work and fasteners aren't always toolbox parts. We use a lot of in house manufactured pins, spindles, and other such fasteners.
Understood. I personally do not like toolbox due to having been burned by it.
I like my own hardware library, so I totally get what you are saying when it comes to patterning
and the toolbox items.
Unfortunately as you have noticed, SW doesn't have a fast, efficent way to accomplish fully defined fastener mating. You either add the 3rd parallel plane mate (not efficient) or live with non fully-defined fasteners.
It would be nice if SW would add a single fastener mate of that recognizes the cylindrical mate and fixes its rotation. Solid Edge does have such a mate- they call it Insert. You enter the mate command, click the (4) surfaces (surface under head and cylinder of both fastener and the part to mate to) and you are done- a fully defined fastener. The mate recognizes the axis of the fastener (or rotating part) and fixes its rotation. Some time back, I pursued this as an enhancement request for SW but didn't get much interest.
this brings up another question I had...Is there a way to tell if all the parts are fully mated?
Lower right corner of your screen.
My two cents
In the FeatureManager design tree, a component name can have a prefix that provides information about the state of its relationships to other components. The prefixes are:
(?) not solved
The absence of a prefix indicates that the component’s position is fully defined. See Mate Errors for information about mate symbols and error messages.
Ignore the emoticons on the minus and plus since above. (I'm not ure how to turn them off and don't care enough right now to find out)
This is from SW help
Assemblies > The FeatureManager Design Tree in an Assembly
Maybe I misunderstood Jim's question. I thought he wanted to know if all components of an assembly are fully defined. Your method is for individual components.
You answered Jim's questions perfectly, I thought.
I just extrapolated a little, but that may have not been necessary.
Yes questions were answered beautifully thanks again!
I am making an assmebly of an elevator,so it includes a no. of parts and I have to change them time to time. So many times my assembly gets under defined, but I canr get which part is not fully defined, so how do I found in an assembly which component is not fully defined
When a part's position in an assembly is not fully defined, it will have the in front of the part name in the tree.
But I don't find any symbol in my tree,I mean not even for fully defined or under defined.
It's not actually a symbol as shown in the posts above.
It's a minus sign enclosed with brackets. ( - )
It shows up here as that is the shortcut used here to give
Thanks A lot man...
The concentric mate has an option called lock rotation, just check the chekbox when mating the fastener:
Alternatively, you can RMB on the Mates folder and lock or unlock all the concentric mates in one go.
Did not know that - great tip!
An often overlooked tool is Assembly Visualization. This is found on the evaluate tab. There are a lot of properties that you can select from by clicking on the arrow on the right hand column to expand a menu of additional selections.
Hey I have a doubt,when I export the flatten piece of a sheet metal part, It have bend lines in dashed format but there is not difference in Up and Down bends, both are shown by dashed lines, It creates a lot of confusion,Is there any way to get over it..
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