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Change length of fastener (from library)?

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Message 1 of 21
tomae
460 Views, 20 Replies

Change length of fastener (from library)?

Is there an easy way to change the length of a fastener I added from the fastener library?  

 

I added a 7/16-20 Ansi Socket Head Cap Screw and the length I needed, 1.125", was not available from the list.  I added a 1" long screw instead.  I want to edit the model screw to add the additional .125" to it.  I don't see parameters that I can change for that.  How would I go about doing that?

 

-Tom

 

20 REPLIES 20
Message 2 of 21
jhackney1972
in reply to: tomae

Since fasteners are generated as parametric models when you ask for them and then placed in the Fasteners Project as a linked file, you have to go there to modify it.  The video will show the process.  This method, or course, is only if you want the screw to remain and be usable in the Fasteners project.  If not, just Break the External link and edit it in the assembly via the timeline.

 

Edit: When you have the fastener open, you can go to the Parameter table and change the value of the variable if you desire instead of typing the length in directly.


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 3 of 21
tomae
in reply to: jhackney1972

Thanks, that is exactly what I wanted.  One question, is there a way to rename it?  It has the length in its name (1.0" in my case) and I want to change it to 1.125"...

 

I should add that I can't seem to change it's name in the data panel where I'd normally be able to Rename a design...

 

 

-Tom

 

Message 4 of 21
jhackney1972
in reply to: tomae

While you have the Fastener open, to change the length, do one more step before saving to rename it for the parts list in the drawing.


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 5 of 21
tomae
in reply to: jhackney1972

Hmm, ok that works.  I hope this won't cause me issues down the road, where a screw is named one thing but has a different description.

 

Thanks for your help,

-Tom

 

Message 6 of 21
jhackney1972
in reply to: tomae

Here is an easier and "more complete" method of changing the Part Number of a fastener and well as the Description.  Do it as you are placing the fastener at the bottom of the dialog box.  You can copy and paste between the fields.  NOTE: you will still have to open the fastener to edit the physical length.

 

Rename Fastener.jpg


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 7 of 21
tomae
in reply to: jhackney1972

So, this already causes me a problem.  

 

I have used the 7/16-20 1.0"lg SHCS in other designs.   So, when I put it into this latest design and changed it's length, and description, all the other designs that contained a 7/16-20 1.0lg screw now had 7/16-20 1.125lg screws (with the wrong part number, but "right" description), however in the other designs that screw is too long.

 

So, modifying a fastener is fraught with danger if you've used it before.  I need to go back and fix the original fastener length and description, and then open another one, break the link, and THEN edit it's name and description (if that's possible) and edit it's length in order not to screw (no pun intended) my other designs...

-Tom

Message 8 of 21
tomae
in reply to: jhackney1972

Well dang.  It's really confused now...

 

So I have now deleted all uses of 7/16-** fasteners in all my designs.  Then I tried to delete the 2 (not sure why I have 2) 7/16-20 1.125lg screws from my fastener library.  Even though "Uses" and "Used In" for both fasteners show empty (both in Fusion 360 and when I look at them on the web, and I have verified and re-verified that I am not using them anywhere, Fusion won't let me delete those two fasteners from my library and says they are referenced by drawings.

 

I need to get work done so I am just going to go back to my old method of building my own library of fasteners from McMaster and forget this thing until it gets sorted out.

-Tom

 

Message 9 of 21
jhackney1972
in reply to: tomae

There is a simple solution to this issue.  Before making ANY changes to the fastener, right click on the fastener,that will be odd-ball, and Break the Link.  This will make sure the fastener, and its modification is ONLY in one file where it is needed.


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 10 of 21
tomae
in reply to: jhackney1972

Right, that would have been the solution ...before I got into this current situation.  Now I have 2 7/16 screws in my library and whenever I insert a new one I get one of those 2 with the wrong part number and/or description (one of them has no part number).  I can then of course break the link and fix it, but that kind of defeats the convenience of the whole fastener library for that fastener (which I use quite a bit).  I will have to contact support and see if they can remove the two screws that won't go away...

Message 11 of 21
jhackney1972
in reply to: tomae

You can also solve the issue of the "Rough" fastener by removing it from the Fasteners Project.  Browse to the fastener you modified, in the project, delete it.  The next time you create a fastener of the deleted size it will be regenerated anew.

 

Edit: Before you do this be sure to Break the Link in the assembly it is used in, the odd length fastener I mean.

 

Delete Fastener.jpg


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 12 of 21
tomae
in reply to: jhackney1972

There is no link to break because I have removed it from ALL of my designs.  That's my current problem.  The fastener is not used anywhere, and yet I am unable to delete it.

-Tom

 

Message 13 of 21
jhackney1972
in reply to: tomae

If you cannot delete it, from the folder I showed you, I assume it says it is used as a Reference in another location.  In this case create a new Project called Trash,  you need it for sure, and right click on the fastener and Move it to the Trash project.  You can Archive the project later on if needed.

 

Move to Trash.gif

 


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 14 of 21
tomae
in reply to: jhackney1972

Creating a fake trash project and moving both of them there worked.

Thanks,

-Tom

Message 15 of 21
tomae
in reply to: jhackney1972

I had some time today and am trying to figure out this "odd size" fastener editing.  I am starting over fresh (after having deleted the other rogue fasteners I created).  My goal is to select a 7/16-20 1" LG SHCS and then edit it to be 1.125" LG and also have that in its part number and description.

 

Method 1:

 

Insert -> Insert Fastener ->  Select Bolts and Screws -> Socket Head -> Hex Socket Head Cap Screw (ANSI B18.3-2003) Then select these Parameters:  7/16, 1.000in, UNF (20 pitch) and THEN edit the part number and/or description names to change the "x 1" at the end to be "x 1.125",  and finally place screw.  THEN I go to Fasteners in the design tree and break link for these two fasteners that I just placed.  

 

Before even editing or doing anything else, the problem with this sequence is if I now select this same screw from the Insert Fastener function (in this design or any other) it has "x 1.125" for the "x 1.000" fastener in it's part number and description.  So this isn't good.  Scrap this and try....

 

Method 2:

 

Insert -> Insert Fastener ->  Select Bolts and Screws -> Socket Head -> Hex Socket Head Cap Screw (ANSI B18.3-2003) Then select these Parameters:  7/16, 1.000in, UNF (20 pitch) and THEN place screw.  THEN I go to Fasteners in the design tree and break link for these two fasteners that I just placed.  

 

Ok, the fasteners now automatically move themselves from the Fasteners folder to be 2 separate parts in the normal (lower part of) design tree.  That's fine I guess.  I would rather be able to create a new fastener in my fastener library that I can use later, but one issue at a time.

 

But now for those new screws in my design tree  "Open" and/or "Edit in Place" are not options when I right-click on these parts now, not sure why that is...    It turns out I can however edit the sketches of the fastener.  It also turns out that when editing the design BEFORE breaking the link, the length was the first Parameter in the list (named adsk_nomlen).  After breaking the link apparently a whole new set of the same parameters are copied N times per instance of screw, so for the first screw, the length is now a new parameter called adsk_nomlen_2 further down in the list.  And for the second screw the length parameter is even further down called adsk_nomlen_3.

 

Also, I can edit the fastener name in the design tree, just like any other part and fix the length in the name there.  However, if I look at the Properties for each of these items the Part Number and Description are the old (incorrect) name with "x 1" in the name 😞

 

So I now have a model that has the correct length fasteners with odd identifying information associated with them.  

 

Before the new Fastener Library feature I had been accumulating (from Insert McMaster-Carr Component) screws that I use in a separate project.  When I use those, I have to place in current design and create a Joint.  I like the (relatively) easy lookup and placement of the new Insert Fastener function, but if it doesn't contain the length screws I need, or or is missing screws I need (there are NO set screws in the fastener library, for example) then I need to jump through these hoops to use it.

 

Seems like this feature should have been a Preview feature or optionally turned on/off since it is currently half-baked.  The last thing I need is inconsistency in my designs so I have to spend time trying to figure out where/what screws are in a design, what they are called etc.  Am I off-base and missing something here?

 

-Tom

Message 16 of 21
jhackney1972
in reply to: tomae

I have created a video outlining the method I would handle Custom Fasteners so the custom ones and the ones generated by the Fastener routine can exist together.  The only thing I did not show is how to capture the custom fastener into you database is you want to keep it to use again but I think that is obvious to you.  I made a little blip in the video where I did not activate the top level assembly but I think I demonstrate how the process works and how it will not "contaminate" your fastener database.

 

In


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 17 of 21
tomae
in reply to: jhackney1972

I like your method, and I'd click accept but I have one issue where it doesn't behave as in your video.  I have deleted all uses of this screw (the 7/16-20 SHCS 1") from my designs, and I have removed this screw from the Fasteners folder.  I have killed and restarted Fusion and verified the fastener is not in my fastener library and not in any designs or drawings.

 

Now, when I insert one of these, then break the link, then activate it, and finally go to Modify -> Parameters, there are now 4 sets of parameters (see screenshot) and I have to figure out which one actually changes the length of the screw.  At this time it is the 4th (last) set.  Not sure what is going on.  It's as if every time I break the link Fusion saves a new set of parameters for that screw or something...?   This isn't a show stopper but changing multiple entries and watching to see which one ACTUALLY changes the length is annoying.

 

-Tom

Message 18 of 21
jhackney1972
in reply to: tomae

If you insert a linked file, containing parameters, then break the link you get a set of parameters in the table.  Insert the same linked file and break the link you will get a second set of parameters with a “_1” added as a suffix.  Repeat and the suffix is increased by 1 to “_2” and so on.  This why  I only inserted 1 fastener before I use the Break the Link command.

I invite you to create a new assembly and try this to see the parameter suffix increase.  Without seeing your assembly, I cannot tell what you did differently from my method used in my video.

 

I will leave this  question as I have presented my best methods for handling custom fasteners.


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


Message 19 of 21
tomae
in reply to: jhackney1972

Ahh, I see now.  Once you insert a fastener (of any type) and break its link, ALL other subsequent fasteners, where you break the link, will create an additional set of parameters (ad infinitum).  Even if you remove ALL fasteners (both fasteners and broken-link fasteners) somehow Fusion remembers that you once had them in this assembly/design and continues to add parameters.

 

Well, this horse is certainly well beaten!  I appreciate your effort to help and explain the behavior.

I may try to use this for a few designs and see what happens along the way.  It is not ideal for me.  It turns out for my specific case that I do, in fact, use many fasteners that are uncommon in thread pitch and/or length  (I'd like a 3/8-20 option for example, not in your library).   

 

-Tom

 

Message 20 of 21
jhackney1972
in reply to: tomae


@tomae wrote:

It turns out for my specific case that I do, in fact, use many fasteners that are uncommon in thread pitch and/or length  (I'd like a 3/8-20 option for example, not in your library).   

 

-Tom

 


My Library?  You must think I work for Autodesk, I am just a user like yourself.  I have no control on the development or what is included in Fusion 360.


"If you find my answer solved your question, please select the Accept Solution icon"

John Hackney
Retired

Beyond the Drafting Board


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