User feedback on Creo2

Hello Elliot,

I can tell you that there is a very good chance that PTC personnel will see this.

For your first six points, the majority of the corporate world would probably disagree. Many of this functionality derives from database management requirements. Most of this functionality actually makes things much quicker and more robust for the user.

• Agree with you on "Windows switching". Creo 2 functionality for switching windows kind of sucks, at least with Win 7.
• Hide/Unhide behavior...I'd rather it be temporary if done from model tree and controlled from layers
• Don't take away my center click. It's been the same since Rev. 16 and I'm happy with it
• Allow for window switching...never been a concern for me
• Allow for mixed Inch/Metric Units...could be a "nice to have"

The proper method for your observations is to post them in the Ideas area. You have to have active maintenance to access this area. PTC is notified of the posted Idea and maintenance users get to vote on it. Several of your observations have already been included in the ideas area so you may want to search for them and vote for them instead of posting it again.

Thank you for taking the time to post your observations. I suspect many of us would really like many of them. Some of the seasoned users understand where the limitations are derived from and agree that the 21 century is upon us and UNIX is something that most people have never heard of (no, it is not a sultan's harem guard!).

So if you do have an active maintenance account, please feel free to post each suggestion in the Ideas section.

Elliot,

Like any CAD tool, the more complex your design and deliverables become, the more you need to know about the tool. I have seen one of the assemblies you are working on and it is quite complex. I can completely understand that without much training or in-house support resources, you could become frustrated from time to time. If you were at a company using Creo as their main design tool, you would likely have access internal support, peers, best practices and previous designs to use as reference.

I would also note that many of the frustrations you are feeling are data management related. Windchill Project Link was developed specifically to address these issues. Anyone not using Windchill or another data management tool has to be very regimented about where files are saved to and how they are accessed.

Below you will find my comments to your list:

• It should always be possible to select where to save. Currently, if a new part,drawing, etc. is made, it MUST be saved in the folder of the last file I opened. The options to put it elsewhere are greyed out.

Josh explained this well.

• Closed files should be cleared from the environment. Currently there is a massive memory leak. Even if you close a file, it is still in memory so long as Creo is. If you are forced to move a file due the having saved it in the wrong place, need to reuse a name of a file that you stopped making or did not save, etc., you have to completely close creo and open it again because the name clashes with the closed version. Also generates a huge memory footprint that cannot be reduced without closing and restarting.

Many users would be extremely upset if closing a window meant their model was remove from memory. The erase tools found in File> Manage Session should be used to manage which models are open in memory and which are not.

• There is no way to tell whether you have saved a file or not. You get a warning that anything unsaved will be lost when you go to close the last creo window, but nothing when you close individual files. Files need to be treated individually, not as a monolithic session, particularly since there is no way to tell creo to save all versions in memory if newer than saved versions from this last window.

I am used to seeing this in my title bar because I typically work with Creo linked to Windchill. It is unfortunate that it is not visible when not using Windchill. That said, if an open part or assembly is saved, it will be saved whether the model has been changed or not. If an assembly is open and saved, by default in Creo, only the assembly and any modified models will be saved, not all the models. You can use Save a Backup to save every component in an assembly to your current working directory or a new folder.

• There is no reason to make a completely new file every time you save something. Embed the old versions in one file as history data, with an option of how many versions to retain. Combine with change tracking and save on close so that saving multiple times without changing anything does not cause older version to be moved off the end of the save queue. This will drastically lower the amount of space taken up by creo work, as each file will be only the current version plus a small amount of data for backtracking, instead of the entire file repeated over and over. The current model causes major problems with windows file handling, since adding '.#' to the end of the file extension leaves windows unable to handle opening anything. It also takes up massive amounts of space and, if using an online storage system, bandwidth, since a complete, full size file must be saved and uploaded each and every time. Exacerbated by having to save repeatedly, in order to make sure you have remembered to save before you close the window, since there is no way to tell whether you have or not

Again, this functionality has been in Creo since the very beginning and is something that experienced users value greatly. If you are worried about your file count or disk space, I would suggest adding the internal purge.exe utility to your Windows Explorer right-mouse pop-up menu. Also, with a little searching, you can find a 3^rd party tool named Spekan Purge. This tool, among other things, enables you to purge a set number of revisions (for example, keep only the last three saved models).

• Open files from the windows browser in the current session. Currently, if you open a file from a folder, it starts an entirely new Creo instance. Files should open in the current instance at all times.

You can drag a model from your windows browser into a Creo window. This will not open a new session.

• Files incorporated into an assembly from a different folder should be properly loaded into the assembly on reload. Currently, any file not in the same folder and an assembly will be missing every time the assembly is opened, requiring manual relocation. This is even true if the file is in a subfolder of the folder the assembly is in. Manual library tinkering can be used to fix this, but it should be automatic.

Again, Josh has explained this well. If not using Windchill or another data management tool, search paths can and should be used to manage common or shared models. This is a Creo strength, not a weakness.

• Window switching should change focus, or creo should be one window. Currently, even though creo creates a separate window on the taskbar for each open file, clicking on the taskbar icons does not change focus; the in program pulldown menu must be used. This completely defeats the purpose of having multiple windows. Either enable switching with the taskbar (preferable), or have Creo occupy only a single taskbar icon.

I too sometimes wish I could active windows from the taskbar. However, with large assemblies, I find it useful that I can view (pan, spin, zoom, etc) an open window (from the taskbar) and not activate my large assembly. If you mistakenly try using the taskbar (as I do from time to time), it’s easy to activate it using the Windows drop-down menu.

• Allow for showing and hiding of axes, planes, etc. on individual parts in assemblies. To do this currently, you have to spend a large amount of time creating layers for each part to do this. It should be an inherent property of the assembly instance.

The default layers included in the PTC template models enable you to do this. The display of datum features in designs throughout the world are managed using this functionality.

• Properly remember Hide/unhide behavior on save in assemblies. Currently, if an item is hidden when the assembly is saved, unhiding it and resaving will not result in it being unhidden when the assembly is reopened. Only manually refreshing the tree and then resaving will permanently changing the state.

As a designer engineer, sometimes I often change layer displays that I don't want saved. That is why we have the Save Status button in the View tab.

• Do not exit modes with center click. Center click (mouse wheel) is used to change view, but also exits many modes, such as 'Edit Definition'. This creates multiple instances of inadvertent exiting of these modes while trying to move.

This has been a feature in Creo-Pro/E from way back (it was a user requested enhancement). Anyone using Creo to make a living would scream foul if this was removed.

• Allow for window switching while in feature specification mode. For example, if creating a hole, it should be possible to start the hole, jump to another file to position or size information, then jump back. Currently, one must completely abort the hole, switch files, and then restart. Especially annoying if multiple parameters need to be taken.

You can only perform/edit one operation at a time. I am not sure how this would be managed if a feature were able to be in a state of definition in multiple windows.

• Allow for mixed Inch/Metric units. Being able to specify dimensions for a part in both will vastly simplify making mixed parts, as well as produce better quality drawings. Currently, one must simply perform the conversion outside the program and hope there are enough decimal points to achieve the needed accuracy.

Agreed, this would be nice, especially for standard inch sized holes in metric unit components.

Additional items:

• Holes and hole patterns should list size and screw type on the feature tree. Currently they are just 'hole_#' or 'Pattern_of_Hole_#'. You have to open the feature up if you want to check the size. Having a listing such as 'Hole_4-40' or 'Pattern_of_hole_0.31' would speed work considerably.

• It is very hard to get the dimension you want on drawings consistently. I often get edge to edge dimensions on holes when I want center to center (or edge to center), or radius when I want diameter. Even when you get this things do not update properly in all cases, such as diameters still having an 'R' prefix.
• Holes must be entered on drawings manually, since the dimensions the program gives are not usable as easily read specifications, as they do not indicate to humans things such as clearance vs tapped holing, counterboring, thread count, or size in a standard way. Having a diameter printed on the hole does not tell a human that it is size 8 tapped. An automatically generated note such as "6x 8-32 tapped counterbore" from you patterns for human readability would save time and prevent errors form having to manually manage notes.
• Allow for inversion and rotation in drawings. Sometimes you have a part model oriented upside down or sidewise relative to the way you would like it to appear in the drawing. This can occur if, for example, you have to add a feature to a part after adding it an assembly, and that feature happens to be on the bottom relative to the original file orientation. Currently you have to redo the part, then redefine the assembly relations. Just let us change the drawing orientation instead, as there is no actual CONTENT change needed. The initial choice of coordinated in the model is not always the most ideal for a drawing.

Also a bug report:

• The mirror feature type often fails to regenerate properly. I find that if I change a parameter of the original item the mirror will vanish, move in a completely unrelated way, or just vanish entirely, rather than regenerate. I almost always have to delete and recreate the mirror to get the feature updated properly.