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How to clear the audit trail history on the model.


How to clear the audit trail history on the model.

Dear All,

May I know how to clear the Audit trail history from the model?




If you are refering to the trail files, I recommend a setting in for placing trail files in a particular folder. That way you can easily delete the content of the entire folder.

trail_dir <drive and full path name>

example: trail_dir C:\PTC_trailfiles\

If you are refering to the history maintained in parts and assemblies, I do not know if we have access to that.

Thanks Antonius!

I am on same way as you have mentioned , so that we can setting up up config .pro on each time and set the start up directory on the same folder.

here , I am facing a problem to delete the model history. (Info---> audit trial) . I am sorry to mentioned that I am using WF-4.


Best Regards,


Thank you. Now that I am aware of this, it is indeed annoying. I see no options in Creo 2.0.

Looking forward to learning how to cleanse these files, particularly for template parts and save-as parts.

Hi guys...

Sorry I haven't been around. The audit trail is a very old tool that most people don't know about. It knows all... and blabs it all, too! There's no way to wipe out the Audit Trail of a Pro/E file through any normal means. What I mean is... there's no button or simple function to 'cleanse' your part.

To me, this is a good thing. I've gone to numerous companies and ran an audit trail on their hardware library or their start part. Usually I can find a few names in the audit trail I recognize. You can see who ripped off other companies for their library parts. You can also see how some expert users hopped from company to company bringing their start parts along with them.

Anyway, let me get to your question.

When you start a file from a start part, all you're really doing is making a copy of an existing part and then opening the copy for modification. As expected, this keeps the audit trail going. If you start a brand new part with no template (literally a blank part), your audit trail will be clean.

Most people don't even remember how they went about setting up their first template part. Way back when, we didn't have "start parts" and some people would just run a mapkey to set up views, add default datums, and load blank parameters. That old school knowledge is gone for the most part but you can use it to erase the audit trail.

Open a new part without using a template. You'll have a clean part. From here you create default datums and add parameters. You can also create your initial views. Save this new object as your new template (so all future parts will start out clean without a long audit trail history). If you have an existing object you want to cleanse, you can create a new part using your new, clean template and use Edit->Feature Operations->Copy->From DifModel or FromDifVersion to pull in all of the features of the existing part.

With a few mouse clicks, it's possible to migrate all of your features from your existing "dirty" part to a brand new "clean" one thus eliminating the audit trail.

In Wildfire 5 and up, the audit trail has changed to the File History command which has additional features. If I'm not mistaken, I stumbled upon some way in either Wildfire 5 or Creo to quickly wipe out the file history... maybe using a copy through Windchill? I'm not sure right now... but given that you're on WF4 it probably doesn't matter just yet.

I realize this is short on details. Write back if you get stuck or if you need help. I've been intolerably busy lately but I'm almost ready to wind down for Thanksgiving. At least I have a one-day reprieve!!

Take care...


Brian, as always... YOU ROCK! I will have to try some of these things. My biggest problem with seed parts has been creating -real- ISO views and needing to create geometry to do it. If only we could import view orientations Maybe your method will do this.

I do see however from your discussion that there is a negative to all this history, specially if you are not aware of it. For us contract engineers, of course we use start parts to prepare for other clients. One could incidently give away what may otherwise be contrued as "proprietary". Definitely something to keep in mind.

Even though you are busy, which isn't neccesarily a bad thing, I am very glad you could provide us with your insight on the subject. Happy Holidays!

So much for that idea... in Creo 2.0 I open an empty part and was able to Get Data/Copy From and all the history came with... good news, so did my view orientations

This option was only available when the part was 1st created. Need to learn more about this.

Nice to know I can start from scratch however. Never tried using an empty part.

I tried this and it works... but you cannot use the Get Data/Copy From function. That brings everything including the history along with it.

  • Open the part you wish to copy from (we'll call this the "existing part")
  • Start a new empty part (no template).
  • In the new part, create defaul datums by going to Datum->Offset Planes. When prompted, enter "0" for the 3 offset values. This will automatically create a coordinate system and 3 planes.
  • In the new part, go to Model->Operations->Feature Operations->Copy->From DifModel->Done.
  • Switch windows to the existing part and click it. You do not have to Activate the existing part- you just have to click it.
  • Select the features you wish to copy. In this case, you want everything accept the first 4 features (assuming you have 3 datum planes and a coordinate system as your first 4 features like most users do). Select the first feature after your default datums, hold down SHIFT and select the last feature in the model. This will select all features.
  • With all features (except the default datums) selected, select "OK" or hit the middle mouse button.
  • Select Same Dims->Done
  • One by one reference planes will highlight in RED on the existing model. Your job is to see which plane is being highlighted, then switch over to your new model and pick a corresponding plane. Do this for all 3 reference planes.
  • Once you've selected the planes, you're shown an arrow on one of the planes with a prompt to choose FLIP or OKAY. Swap back to the existing model to see what the arrow looks like. Mimic the direction on your new part (flipping the arrow if necessary). Hit OKAY when it's facing the right direction. Repeat for the second directional arrow.
  • If all has gone correctly, you can just select Done from the Menu Manager and then Done again. The features will be copied into your new model as one large group.
  • Select the Group from your model tree, right-click and select Ungroup. Your features will cascade into the model tree.

If you check the File History after performing this step, you'll see it's very bare except for the copying of features you just performed.

If you're wondering WHY all of this information is now being stored in the File History, just go to Tools->Investigate->View Changes. You can see every change that's been made to a file since the start of the session (there are other options, too). You could never do this before Creo.

This technique requires using very old tools that have been carried over from the very, very old days of Pro/ENGINEER... circa v.13 or so (1994 ish?). The procedure is a little cumbersome (it's always been that way) but it gives you the power to pull features from another part in a very convenient way. By using this in conjuction with a new part, you can defeat the File History.

There may be another way, but off the top of my head, this is what I would go with unless someone chimes in with a more efficient technique.

Happy Thanksgiving! And good luck!!


Ah... one other thing... you don't have to create geometry to create real ISO views. Go to the Reorient command and select Dynamic Orient from the very top drop down box. With the red/green/blue gimbal icon pushed in, rotate -45 degrees in the vertical axis. Switch to the other icon (the one next to the red/green/blue gimbal), this is screen orientation mode. Rotate in the horizontal axis -35.266666 degrees. Save this orientation as Isometric.

It's totally possible to set up a new part with all the appropriate named views using one mapkey. We used to do this all the time before start parts came along.Today though, you only need to do it once and save your new template file. In Creo 2, the system automatically recognizes the TOP, FRONT, RIGHT, LEFT, BACK, and BOTTOM views to help with placement of annotations for model-based (paperless) definition.

Anyway, hope that helps!!



I remember that you could not give the angle in less than 1 degree increments... that must have been fixed. BTW... it is 35.2644 from what I remember of the ol' days

I still prefer to make it exact by using the corners of a cube. Call me strange

Nah, it's not strange. Whatever works, right?

You should make a really great new start part with the perfect isometric views and post it here. It's amazing that after all this time, someone hasn't started a repository to share useful models like this.There are websites out there where you can post models but nothing easy to find or use.

Wait... scratch this entire idea. I'm stealing it for myself!

Seriously though... why don't we have this? Hmm... maybe it's time to send Dan an email!

Dear Brian,

Thank you so much for so elaborated reply. At present i am gioing withe method as you have mentioned. i was just curious to know about the clearing audit trail.! so i thought of sharing my qurey to experts like you.

Thanks Again for your precious time!

Kind Regards,


I still think there's an easier way and I feel like I've stumbled upon it before. I either cannot remember it or I am mistaken that there's another way. If I ever figure out another way, I'll add it to this thread.

Take care...


Something seemed to have happened in Creo 2.0 M030. The only history I see in the model is save events. No more history for feature operations and no more viewing options. Anyone else having the "new" behavior?

Someone please post an image of the older screen that shows all operations and buttons so I can report this...

tools/investigate/file history


In Creo 2.0 M020 it seems to work. See the attachment.

I didn't bother switching to M030 yet.

Thanks Jakub. I will report this.

Jakub, can you post the full HTML window? I think some buttons are also removed.


I take it you decided to update your maintenance. Wait for M040 coming out soon. M030 is pretty buggy compared to M020.

hi Tom,

Check your email.

Thanks Jakub. It is the filters that are also missing. The case has been forwarded to PTC R&D as an SPR. I'm thinking someone messed up the web app. This should be an easy fix but this scary how something so simple just gets hosed.

A simple but hack way of doing what you want is describerd here:

Thanks Dan!

I know this is an old thread but an update is warranted...

Today I received an update on my case about the missing file history and not what I expected.

According to CS, the way file history works today is what it was meant to do. Very simple saved, saved as, etc data and not the detailed data you saw in Creo 2.0 M020. Bummer!

For anyone keeping track of CS response time, this is a -fail-, 3 months and 2 updates before they could answer this simple question. And the answer isn't what I expected. Seems detailed file history is not as important to PTC users as it is in every other CAD package in the world.

hidden config option:

purge_history_on_save_copy set to yes

Save your model as...

The new model will not have the purge history

overwrite your old one with the new one.

This may cause some issues, but at least you don't have the history.


Nice! When was this added?

based on google's limited results on the option, I'm thinking Wildfire 5.


It was introduced in Creo Elements/Pro 5.0 M130.

Thanks Mahesh. Any side effects we should be aware of in using this option?

Side Effects? Yea,

But don't think that just removing the file history/audit trail will prevent files from being traceable from one company to the next.

It's not worth 10 plus years of your life in court and all the costs and hassles associated with it, I would recommend just take the day or two to re-create from scratch OR get your start models from a public source.

Google "Eaton v Frisby" if you want to know more.

yeah... for me, I think the best use of it is to clean up the start parts file history from all of those tweaks over the years. Other than that, I would keep the history for legal reasons.

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