Skip to main content
BrianMartin13-Aquamarine
13-Aquamarine
August 16, 2013
Solved

Creo 2.0 Drawing Performance Issues

  • August 16, 2013
  • 24 replies
  • 21732 views

Hi Everyone...

I have to be brief but... does anyone else have really bad performance issues in Creo 2.0 when working on a large assembly? Build code can be M040, M050, or M060. It doesn't matter all three are similarly bad.

I have a 4-sheet drawing with a rather large assembly. There are tons of "lines". Simple operations like zooming in/out, moving a view, and even just selecting an object are taking forever. I've tried every trick I know and it's as slow as it can be. When I click a dimension to move it and Creo takes 5 second to select the dimension, that's bad.

Imagine this scenario... I need to more a tiny detail view a few inches to the left to make room for something else. I move to the view... 3 seconds later, it highlights. I click the view... 4 seconds later, the drag handles activate. I hold down the mouse button and drag the view... then let go of the button to drop it. Creo takes 20 seconds to move the view and repaint. Moving a view just took 30 seconds.

Now imagine I have 100 items to balloon and dimension... and pages of details yet to complete. What the actual *! $^#( is going on? Just a simple zoom isn't possible. I roll the mouse wheel... 2 seconds later the view updates. I roll again... one little notch on the wheel... and 2 seconds later, the view updates.AHHH! I'm going to lose my mind.

Oh- here's a neat trick... activate the Merge Balloons tool... and suddenly the views zoom normally again. So now when I'm zoomed in tight to a detail and I need to zoom out a little... I hit a mapkey to activate the Merge Balloons tool and I can zoom around again. Then I deactivate the tool and go back to work.

Any ideas? Similar experiences?

Thanks!

-Brian


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.
    Best answer by dveljkovic

    Brian, try to deselect "enable preselection highlighting". Maybe Creo is trying to preselect detail below the mouse pointer hence the wait.

    24 replies

    JamesBurcham1-Visitor
    1-Visitor
    August 16, 2013

    I had a similar experience. My issue was that my parts had tens of thousands of features, so regeneration time was slow. Its possible you are having the same issue. We spent plenty of time working with PTC, but the only real solution was more computing power.

    BrianMartin13-AquamarineAuthor
    13-Aquamarine
    August 16, 2013

    Hi James...

    I'm working on a brand new workstation with 32GB RAM, a 2GB graphics card, and screaming processors. I wish I could chalk this up to processing power. The trick with enabling the Merge Balloons tool seems to suggest that greater speeds are very possible... but that something inside the Creo code is causing the slowness.

    Oddly though, usually processing bottlenecks do show up at regeneration time. My model regenerates quickly... but the drawing is just like running in molasses.

    Thanks...

    -Brian

    TomD.inPDX17-Peridot
    17-Peridot
    August 16, 2013

    Brian, you are likely dealing with the GPU regen issue (not considered an issue by PTC). Even on a very simple model, I can get similar behavior.

    Turn down the shade quality; turn off the textures; turn edge quality display to low; and turn off anti-aliasing.

    Even if you don't have shaded views, I suspect the GPU regen goes through the entire file to refresh its filtering index. It seems to be rebuilding the entire polygon database between every command.

    It is almost like we need to go back to the limited CPU days where we have to turn off views to make it interactive. Oh, yes, that too may help get the ballooning done.

    BrianMartin13-AquamarineAuthor
    13-Aquamarine
    August 16, 2013

    Thanks Tom...

    I'm not using any shaded views on the drawing. In fact, I tried adding a few to see if the shaded graphics performed better. In model mode, shaded models have traditionally been the fastest. Well, unless you want to go back to the way things were in 1995 when wireframe was fastest.

    When I turned shaded views on... things got exponentially worse! I've already tried several of the options you've suggested. I didn't consider messing with the shade quality settings or texture settings because I'm only doing "no hidden" views.

    I also hadn't tried Danilo's suggestion (below) because the preselection didn't seem to be the core of the problem. Once I had already selected something, it still took forever to move it or to right-click to work with the object.

    But... since you guys brought these issues up, I went hog wild and turned off every single shade option I could find and the preselection highlighter. What do you think happened?

    Total failure, right? Amazingly... it sort of worked! The only problem now is figuring out which of the 25 options I just toggled had the greatest impact. I wouldn't call the performance impressive or anything... but it's usable which is better than wasting hours tediously messing with this drawing.

    I'll see if I can isolate the problem...

    Thanks for the suggestions!

    -Brian

    TomD.inPDX17-Peridot
    17-Peridot
    August 16, 2013

    Shading is only an artifact of how PTC has been doing graphics processing since inception. Everything graphic is done through the facet model. This is what give you "no hidden" views and shading at the same time. This is from the now archaic VRML world. So whenever there is a "regen" of any kind, it rebuilds the facet model.

    So here is part of the rub, even if your high quality image of the model regen's quickly, it does so for every view in the drawing when in drawing mode. And this creates a selection index which becomes "HUGE" because it is picking "through" the facet edges which you never see. I certainly hope it doesn't propagate through all the sheets as well. That would be dumb!

    I suspect you will get better performance if you also use your selection filter. If only we knew exactly how the selection code was working. Part of all that focus on 3D annotation has really left the core detailing functionality in the dust. I worked on one model with textures that was absolutely intolerable. All that was wrong was the display quality set to high. Medium and low was exponentially faster.

    The hint that gave me this idea is how large the files were when saving models with high quality settings. Every single faces, including LOD levels were being saved. This makes each part huge when creating filtering indexes too. PTC has simply lost their edge in managing their graphics engine. What has always been a easy way to manage GPU cycles has become a liability. And the code people have simply ignored this overhead hoping the graphic engine guys would keep up. Guess what... it didn't happen!

    I don't know if PTC is taking this issue seriously. This is starting to cost clients money in productivity. We can only hope that people like yourself can force a corrective course through the right channels.

    dveljkovic10-MarbleAnswer
    10-Marble
    August 16, 2013

    Brian, try to deselect "enable preselection highlighting". Maybe Creo is trying to preselect detail below the mouse pointer hence the wait.

    BrianMartin13-AquamarineAuthor
    13-Aquamarine
    August 16, 2013

    Hi Danilo...

    Wow... believe it or not... it was the stupid preselection highlighter! I don't know if I would've even considered that. I toggle it while working on models but I never tried it in a drawing. It's usually so useful in a drawing that I never thought to turn it off.

    This is the first of the 25 switches (mentioned in the reply to Tom) that I tried toggling to isolate the 'culprit' option. It's crazy that the preselector was causing the problem. That led me to think a bit more about the problem. Why would Merge Balloons also seem to solve the problem?

    Then it all made sense... when Merge Balloons is active, your selection filter is set to exclude everything except BOM balloons. I went ahead and tested this theory but changing my selection filter from General to "Snap Line". This also increased my speed. In fact, setting the filter to anything but General did the trick.

    With General active, the preselection highlighter is looking for all object types. In a drawing with 10,000 lines and annotations, it's getting overwhelmed. By narrowing the preselection filter's choices, you can keep it on and still speed up your drawing work. For the fastest speed... turning it off on large drawings is the answer.

    Thank you Danilo... really!

    And sincere thanks to everyone who replied. Usually I answer the questions but this was a welcome change. Plus, I finally get to award points to someone for a correct answer!

    Have a great weekend everyone!

    -Brian

    dveljkovic10-Marble
    10-Marble
    August 16, 2013

    Brian, you are welcome. I am dealing with these things all the time - every time. In model mode I usually use "datum" filter (instead of unchecking the preselect option) so Creo does not start filtering through parts, edges, surfaces and-who-knows-what-else trying to preselect while I am manupulating with models. Of course, show-plane button is off. And it helps. As for preselect option, there should be an option to use it when some defined key is pressed, like CTRL or ALT or both. In other cases it should be off. We had a macro that was switching preselect option on of off but we do not use it anymore. Have a nice weekend to all.

    Patriot_1776
    Patriot_177622-Sapphire II
    22-Sapphire II
    August 27, 2013

    I can see this, I have turned off preselection highlighting since it was first introduced (I query/select everything), but leve highlighting on in the layer and motel tree........except when I have dwgs with very complicated views (tons of lines), then I have to turn it all off, especially the layer setting.

    gkoch2-Explorer
    2-Explorer
    August 30, 2013

    Yes we had a lot of complains about drawing performance being very bad and it mostly was due to pre-selection highlighting.

    Actually this was on by default in older versions as well (Creo Elements/Pro 5.0 for example).

    But what has changed with Creo Parametric, is that the default selection filter in drawing mode has changed from "Items and Views" to "General".

    In contrast to the old default, "General" includes all model geometry as a possible selection, e.g. all edges - which can be quite something to highlight.

    Besides this: Some improvement to graphics speed is expected by the new config.pro option in Creo 2.0:

    fasthlr_drawing yes

    James621-Visitor
    1-Visitor
    August 30, 2013

    The setting fasthlr_drawing yes will make thread lines/semi-circles on threaded holes dissapear from drawing views.

    Patriot_1776
    Patriot_177622-Sapphire II
    22-Sapphire II
    September 3, 2013

    Hmmm, well THAT's not an enhancement..... I was all set to change that option. Thanks for the warning Jakub!

    KeithMarriott3-Newcomer
    3-Newcomer
    March 11, 2014

    Hi I guess that this is a realtively old post now but I am new here. I would just like to point out that you can toggle fasthlr for drawings on and off using the View tab, there is a button on there. You can set your default to on or off using your config.pro so at least there is no need for a mapkey or restarting CREO as suggested by Danilo.

    Terms & ConditionsAccessibility statement