Fasteners

[346gnu]

Hi,

Why are we allowed to create a preloaded fastener that has neither fix separation OR a contact region? (image1)

The fastener is 'shrunk' (image3) but unsuprisingly, the forces are all zero when the model is run. (image2)

I have only tried this in Creo2.0 M060.

Thanks

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[346gnu]

Steven,

Thanks for the attachment,

every time I ask TS about fasteners they send me this or similar ...

[346gnu]

Steven,

I discovered I didn't have to have either a contact or use fix separation.

I just get the warning that surfaces won't be bonded and it lets me do it.

I would have expected an error forcing me to do one or the other or a warning stating that fix separation will be switched back on because I don't have a contact.

Under what circumstances would it be useful to have neither?

Thanks

[danderson]

Steven,

It was my understanding that with Creo 2 you no longer need to run it a second time as stated in your pdf as PTC has made changes to how fasteners are handled with the Creo 2. There is still the issue that a Simulate fastener going thru 3 or more parts is not supported by any version of pro/e (this is what PTC's top level tech support is saying) even though it seems to work. I see Charles setup involves 3 parts being fastened together.

Don Anderson

[mfischer]

Hi Steven,

You are correct. In Creo 2.0, you still need to run it twice.

The background....when a fastener preload is specified, that amount of load is applied through the 'fastener-spring' to the un-deformed model. As the model deforms, the resulting (actual) preload is typically less than the value specified and is reported in terms of a measure. Based on this information, the user has to estimate a new value for preload that will result in an actual preload equal to the desired value and rerun the analysis. Typically they would have to scale up the preload value and then rerun the analysis.

In Creo 3.0, there is a new option that will allow the system to run the initial analysis, determine the value, automatically scale the preload and re-run the simulation. The result would be that the specified preload force would be what is applied to the deformed object.

Hope this helps.

Mark

[mfischer]

Hi Steven,

There is a new option called "account for stiffness' in the fastener dialog when you assign a preload force. This will tell simulate to run the analysis once......but behind the scene the analysis is run through twice. This option automates what is currently being done manually. I was talking about what is happening behind the scene. For the user, they would just have to run the analysis once.

make sense?

Thanks,

Mark

[346gnu]

Mark,

Last time this was discussed I was interested in the nature of the feedback.

When one runs the studies twice one learns about the stiffness of the surrounding structure. That is, where the preload needs to be increased more to achieve the desired preload implies lower surrounding structural stiffness (or modelling error or design error).

Do you know whether the new preload input required for desired preload output will be published to the summary files?

Thanks

Charles

[mfischer]

Hi Charles,

The Engine will print out measure values in the Study Status Report (RPT file) after the base analysis, as well as the final analysis. That way, you will be able to compare the “fastenerName_axial_force” values and how they converge to the specified preloads. The measure values of the second analysis will be the ones available for result graphing and inclusion in studies.

Hope that helps.

Thanks,

mark

[346gnu]

Thanks for that Mark. That's good to know.

We need to have a clear understanding of which fastener's preload have been unreasonably ramped up which may indicate any number of errors (or possible rookie controlled flight into ground).

Any thoughts my original question?

Regards

Charles

[mfischer]

This is a good question......

When placing fasteners with preload, you really have two options....or you will get the results you encountered, which in most cases is not desirable.

The decision you have to make is accuracy or speed....

1) Fix Separation

• When placing a fastener with preload force, you should first select Fix Separation. This will utilize a linearized contact interface between the two surfaces. Fix Separation works fine as long as there is a good amount (say 90%) of the compression at the interface. Setting the ‘Fix Separation’ ON. If there are warnings in the RPT file (saying that the Fix Separation is not working as expected), then use the real contact interface.

2) Real contact interface

• If you are using a contact interface with friction between the two objects (surface or component), then you would turn off fix separation. This type of analysis is more accurate but will force nonlinear analysis and will take more time to process.

In your example, when you turned off fix separation, the system did not provide a warning, it just stated that the two highlighted surfaces will be a contact surface pair. Now you would need to create how these surfaces should interact. By default they are free...unless you created a contact interface between them. This will provide the proper results you are looking for.

Does that make sense?

Thanks,

Mark

[346gnu]

Hi Mark,

Yes that's sensible.

I was trying to understand whether there would be any circumstances where having neither fix separation=on or contact region is desirable.

If there was no contact region then wouldn't it be better that it be impossible to switch off fix separation? It may take a moment or two for the user's penny to drop as they (me) try deselecting 'fix separation' for the unpteenth time ... followed by a conscious effort at creating a contact region.

Otherwise we could have odd fastener behaviour disguised by the results of a more complex model.

Thanks

Charles

[346gnu]

Mark,

I just had a moment to play with the 'account for stiffness' check box and move on my methodologies that seem otherwise to be stuck in time.

The .rpt does indeed provides 2 sets of measures for fasteners.

The first set of measures is for the fasteners where the desired preload is attenuated by surrounding elastic structure.

The second set of measures increases the preload automatically to account for this attenuation and we get what we require.

In other words, it works.

BUT

The fastener preloads in the fastener definition box are not updated.

The user input fastener preloads required to achieve the required preload (with structural stiffness accounted for) are not listed in the .rpt file. (I realise that these can be back calculated from the info given)

I see 2 pitfalls

1. If a user does not update the preloads entered in the fastener definition dialogue box he must always use the 'Account for Stiffness' function. This means that there is always 2 calculations. If he adjusts the preloads in the fastener definition box then there 'Account for Stiffness' is not required and there is only 1 calculation. This is not a problem for s simple model (minutes to run) or for a 1-off study. But the chances are there will multiple design tweaks and re-runs and the analysis time measured in many minutes to hours. Using account for Stiffness doubles the time.

2. A user must be absolutely aware that if the preloads are not updated, 'Account for Stiffness' must always be used.

I propose that the required input preload for each fastener calculated from 'Account for Stiffness' be presented in the .rpt file with words that explain that unless the fasteners are updated with these preloads then 'Account for Stiffness' must always be used and that this will increase analysis time

A nice to have would be a check box in the analysis definition form

And a diagnostics warning as follows

Regards

Charles

[346gnu]

Don,

My setup is only 2 blocks and 1 fastener (bolt).

The image3 (red/blue displacement) makes it look like 3 only because the fastener length has been changed to make the blocks interfere (by the amount the s/w believes is the required length change for the intial input preload to be generated)

By 'intial input preload', this is the preload desired which becomes less due to surrounding structural stiffness not being infinite... or in my case the surrounding structural stiffness is zero because there is neither separation springs OR contact stiffness.

as an aside, 3 or more components has always worked for us. Just have to remember that contact is (until Creo 3.0) generally frictionless and intermediate components can be squeezed out like bars of soap.

The '1 shot' preload is with Creo3.0. Tad D included a screenshot of what may be ...

http://communities.ptc.com/message/229486#229486