I just opened an assembly design that I had completed about 1 week ago. I added some parts (no smart fasteners), then went to a different configuration to work on a different area of it. Upon getting to that configuration, I changed the added parts to hidden, and the smart fasteners instantly became huge. Has anyone any clue as to why this happened? sw 2003
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Smart fasteners-why would they come in huge sometimes? 1
- Thread starter borsht
- Start date
I don't know specifically why that happened, but I did see something similar. When sharing assemblies with an off-site user, he got the same huge fasteners. It was a problem with his software recognizing the toolbox parts, so they reverted to the generic size.
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The reason that your toolbox parts will come in huge like that sometimes happens when you share data with other people.
Depending on how toolbox is setup.
By default toolbox keeps its parts on your hard drive and when you first install it, it has blank parts without any configurations. When you add a new fastener it opens the toolbox part on your hard drive, creates a new configuration then saves that part and inserts it into your assembly.
This works great until you send your parts and assembly to someone else.
When they open your assembly that contains toolbox parts, it will look in their directory... and if for some reason they have not used that particular size fastener it will not see that configuration in the part and it will default to the blank screw size (usually a 1" x 1" bolt).
The best thing to do in that case is if you are sharing data between users in house is to make sure that you setup toolbox parts on a shared drive on your server.
If you are sending data out to a vendor, to make sure that evrything goes with your project, create a new directory somewhere, then you open the assembly that contains your tool box parts. and saver the assembly, part files, and toolbox parts in a new folder using the refernces button in the saveas dialog box, making sure that they all get placed in that new directory.
Now you can zip them up the intire folder and send out the data.
But like I said IN HOUSE by all means use a common toolbox folder for sharing these files.
Hope that helps
Regards,
Jon
jgbena@yahoo.com
Depending on how toolbox is setup.
By default toolbox keeps its parts on your hard drive and when you first install it, it has blank parts without any configurations. When you add a new fastener it opens the toolbox part on your hard drive, creates a new configuration then saves that part and inserts it into your assembly.
This works great until you send your parts and assembly to someone else.
When they open your assembly that contains toolbox parts, it will look in their directory... and if for some reason they have not used that particular size fastener it will not see that configuration in the part and it will default to the blank screw size (usually a 1" x 1" bolt).
The best thing to do in that case is if you are sharing data between users in house is to make sure that you setup toolbox parts on a shared drive on your server.
If you are sending data out to a vendor, to make sure that evrything goes with your project, create a new directory somewhere, then you open the assembly that contains your tool box parts. and saver the assembly, part files, and toolbox parts in a new folder using the refernces button in the saveas dialog box, making sure that they all get placed in that new directory.
Now you can zip them up the intire folder and send out the data.
But like I said IN HOUSE by all means use a common toolbox folder for sharing these files.
Hope that helps
Regards,
Jon
jgbena@yahoo.com
We are running into a problem with toolbox and no one has been able to provide any answers.
Our toolbox is on the network and is shared by everyone and is not write protected. The problem is is if I insert for example a SHCS in my assembly and then someone else tries to insert one into their assembly then it will not let them. Telling them that it is read-only and will stop. The only way I have found to get it to work is that if the original person that put the SHCS in their assembly closes their file and that seems to free it up for someone else to use.
This is becoming a bigger and bigger pain so any imput would be great.
Our toolbox is on the network and is shared by everyone and is not write protected. The problem is is if I insert for example a SHCS in my assembly and then someone else tries to insert one into their assembly then it will not let them. Telling them that it is read-only and will stop. The only way I have found to get it to work is that if the original person that put the SHCS in their assembly closes their file and that seems to free it up for someone else to use.
This is becoming a bigger and bigger pain so any imput would be great.
Yogi,
What oyu need to do is make a change on everyones toolbox browser to make them insert their parts as read-only...
from the toolbox dropdown menu, click on browser configuration. The go to document properties...
make the follwing changes to the configuration on each users installation:
set these areas as follows:
in the "copy part" region set "NO COPY (always use master part file)"
in the "read only status" area set "INSERT AS READ ONLY"
In the "writing to read-only documents" area set "ALWAYS CHANGE READ-ONLY STATUS OF DOCUMENT BEFORE WRITING"
This will fix your problem.
hope that helps
Regards,
Jon
jgbena@yahoo.com
What oyu need to do is make a change on everyones toolbox browser to make them insert their parts as read-only...
from the toolbox dropdown menu, click on browser configuration. The go to document properties...
make the follwing changes to the configuration on each users installation:
set these areas as follows:
in the "copy part" region set "NO COPY (always use master part file)"
in the "read only status" area set "INSERT AS READ ONLY"
In the "writing to read-only documents" area set "ALWAYS CHANGE READ-ONLY STATUS OF DOCUMENT BEFORE WRITING"
This will fix your problem.
hope that helps
Regards,
Jon
jgbena@yahoo.com
I tested that with another guy here an it looks like that will work. Thanks.
One more question.
When I drag a part out of the toolbox it seems like it takes 20 sec's or so before the dialog box pops up. Do you have any advice on how to speed that up?
Thanks again.
One more question.
When I drag a part out of the toolbox it seems like it takes 20 sec's or so before the dialog box pops up. Do you have any advice on how to speed that up?
Thanks again.
Ummmmm... well not seeing the setup, and not knowing much about the history... I can say that there may be a couple of possibilities... 1'st and foremost since you are accessing the files over the network... it could have much to do with the speed... not enough bandwidth.. slow network interface, or locally the speed of the machine, performance settings... Im betting it's a network issue.
Regards,
Jon
jgbena@yahoo.com
Regards,
Jon
jgbena@yahoo.com
A good way to preserve your assembly and all its component, including toolbox fasteners, when sending it to your vendor, is to use "Find References" command. It can be found in File menu. It will find all the subassemblies, original and standard parts that are used (referenced) in this assembly and save them in the directory (drive) that you specify. Everything will be in its original condition. It can even preserve your original directory structure if you select this option when prompted.
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