Creo Parametric 8.0 - User Interface and User Experience Enhancements (Video 2)

creole parametric 8.0 has a number of enhancements and improvements to the user interface and the user experience the first one that you'll notice is that datum planes by default are shaded now also our coordinate systems appear with a red green and blue appearance if you don't want to see the datum planes being filled if you go to your datum display control in the in graphics toolbar there is a checkbox where you can disable that and then re-enable it if you want to also there are a few other places where we have controls for these if we go to file options and then options and then to our system appearance we can expand the datum group underneath global colors here is a checkbox for the rgb colored axes also if we go to our entity display down here we have display 3d datum planes show datum planes with a color fill and a fill transparency these have corresponding config.pro options and i will show those later on let's cancel out of here the next thing i will show is creating a sketch and some of the changes in there so i will click on the sketch button to go into sketch mode i will just grab a shape from the palette let me go to profiles i'll just grab an eye shape and just drop it in here and then let's close out of there and i'll just hit the check mark over here and let's zoom in and i'm going to turn off the display of my datums now since i do not need them so you can see that we have an improved appearance to our different constraints they appear in a little circle and they have a background color also with the different dimensions on here if i drag the dimensions over into the shaded area you can see that they appear with a background as well to access the controls for these you can go to file options options and then we'll go back to our entity display if i scroll down in the list here we see a bunch of different options for dimensions annotations notes and reference designators and you can see that we have a dimension background you have a drop down list where you can control where the dimension background appears also you have controls over the colors and the transparencies if i scroll down even further in this list we have our constraint display settings where we can control the size and the background color and the line color now for a number of these different controls you do not have a corresponding config.pro option just remember anything that you have in here that does not have a config.pro option will automatically be stored in your ui customization file when you click the ok button alright let's cancel out of here since i didn't actually change anything another control that you have in sketch mode if you go to the setup drop down menu here we have show and you have the ability to control the display of weak dimensions so for example i just turned off the display of weak dimensions hey let's go back and turn their display back on also from that setup show command this is another location where you can toggle the display of a dimension background if you do not want to see it but let's turn that back on you might have noticed that again the dimension that i had overlapping onto our shaded background that one now appears with the background appearance in order to be more easily read all right let's hit the check mark to finish out of this one and now with that sketch selected i'm going to hit the extrude tool and i just want to show you that the dashboards have been updated so the icons are made a little bit more prominent in here also you'll notice when i went in here the placement tab was automatically open and that's another setting that you have automatically where the most likely panel that you're going to interface with is going to be opened by default when you go inside of a tool also as i brought the model tree back you'll notice that the location of the tabs in the panel itself moved over so you'll no longer have that overlapping between the panels and your model tree let's cancel out of here and switch over to a sheet metal part and let's create a flange wall so i'll click on the icon i'll just pick an edge over here and you can see the flange so we have the placement tab you can grab any of these panels and move them around or lock them into different parts of the interface let me move this back one over here or if you just click on this particular button it will attach it to the dashboard back in its original location and one thing that's also helpful is that you could have multiple different tabs open at the same time so for example here i've got the miter cuts and especially in sheet metal when you're trying to control a number of different things hey have as many panels open as you want in here and you can leave those in there and then when you are done you can close out of here if you move these different panels off let me hit the check mark and then go to create another one of those features you'll notice that those panels retain their previous position and whether they were opened so that is another change that you'll see to your dashboards along those same lines let me go back over to that standard part model that i was using let's again just extrude this some depth and hit the check mark and take a look at another example of an updated dashboard so for example if i go to create a hole let me close the shape tab i previously had that one open you can see that the way that the different icons appear on the ribbon are again a little more prominent a little bit different organization than you had in creo 7.0 and earlier let's cancel out of that one and the next enhancement that we will take a look at let me switch to a different part let's grab a part that has some inheritance in it so here i have a part and there is the external inheritance feature down at the bottom of the model tree now i'm not a person who notices icons be aware that when you have these icons with a plus sign on them it indicates that something actually has been varied in the feature let me select the inheritance feature and then use edit definition from the mini toolbar if i go to the options tab and then varied items well a little change that they made to varied items is that you'll have in parentheses the number of different items that were varied and on the different tabs it tells you what was varied it's a little time savings improvement because in career 7.0 and earlier if you did have varied items sometimes you would have to like you know just click on the different tabs and see oh well something changed over here whereas now i know exactly what has been varied i can go right to the tabs with that information let's get out of here and take a look at the same thing for a part that has flexibility so i've got this spring if i go to my model properties again that's an icon that i have in my quick access toolbar then down here we have flexibility and we can see that it is defined if i click the change button here in the flexibility dialog box i can see which tabs have something flexible to find we know that the dimensions there's one dimension that is flexible also from the parameters tab one of the parameters is flexible as well all right let's close out of there the next thing that we'll take a look at let me jump over to a model with a bunch of surfaces and first off if you take a look at the model tree there is now a design items folder here i can collapse it and expand it and in your design items folder you will have your quilts and your different bodies if you go to the settings button you now have the ability to display the design tree as its own separate tree you can see it is to the right of the model tree and again we can see all our different quilts inside of here we can see our different bodies you will notice that the design tree has its own separate search and filter as well so you can search independently in the model tree and in the design tree when you have displayed in its own separate window let me go to my settings for the tree filters a few things that i want to point out first off if you go to the body quilt tab you have the ability to display consumed bodies and consumed quotes in here as well another control that you have is the ability to display custom groups in your design tree let me close out of there after hitting the ok button so now if i right click on the top node i can create a custom group and here we have the custom group and i'm going to rename this maybe i'm going to call this one the fuselage and hit the enter key and then i can grab different quilts and i can see okay here's the quilt and let's grab it and drag it to be located in here so that is a way of getting some additional organization similarly i can create a custom group let's rename this one and i'm going to call it wings and then if i right click i can create a custom group within the custom group and then i can say hey let's make this one the starboard wing and then i can create another group and make this one the port side wing and that way i can have additional organization and controls in there so for example here we have this quilt well let's grab this quilt and drag it this is from the port side so it should be in there and then i've got this quilt hey let's grab this one and drag it in there and add other additional items in here as necessary to organize the different quilts and bodies in the model and one of the reasons that we have this new design items folder and design tree is so that you can organize the model differently than using local groups in the model tree because with local groups that's dependent on the order of the features in here well with the design items you can organize these independently of the regeneration order in the particular model another thing to point out about the user interface take a look at the editing group here in the ribbon now you might not notice this but in previous versions in creo 7 and earlier most these icons were grayed out until you had something selected back when wildfire 1.0 came out back in 2003 there was this concept of having two different workflows you have the action object workflow or the object action workflow i know kind of weird the basic difference between them is that you can invoke a command first and then do something to an entity in your model alternatively with the commands that are object action you have to select something first and then the commands become available and yeah that can be confusing especially for newer users who don't understand the difference for that reason now most of these commands here are available from the get go also i want to show you some of the differences in the interface for these commands first one that we'll take a look at when you click on the trim command now you have the ability to specify the type when you are creating the initial feature so back before the type of the feature was dependent on the inputs that you gave it but now you can invoke the command first and specify whether this is supposed to be for trimming a curve or trimming a quilt similarly let me go to the intersect command so the intersect command can be used to intersect surfaces or intersect sketches choose that from the beginning and also the offset command i did like five videos on the offset command here you can see where you can specify if it's going to offset a surface or you're going to offset a curve or create an offset quilt boundary chain so let's cancel out of that one another thing to take a look at if i go to the view tab now we have a drop down that allows us quick access to the control of different appearances in the model so for example here we have solid bodies we can toggle the transparency of solid bodies in the model only bodies that are flagged as transparent are affected select a body and click make transparent command to flag it also we have our quilts here we have a transparency control with a slider and also controls for toggling the transparency of all tessellated geometry in the model so for example something that you might have brought over in an stl file and the last thing to take a look at in this particular model let's say i want to create a published geometry feature if i take a look in the model we can see that the last two features are published geometry features there are a few other published geometry features in the part this was created back in the day now when i create a published geometry feature let me use the control key to select a couple different surfaces let me go to the properties tab and i'll call this i just like to call them pg for published geometry i'll call this wings now when i hit the check mark if you take a look down at the bottom publish geometry features are created in the footer of the model by default one other thing to mention about the design items here i have a body merge feature in another video i showed how you can use patterns of different references in your boolean operations now i'm going to cancel out of here i just want to show you that if i expand bodies well then we have the consumed bodies appearing in here as well in a different color if i go to my tree filters once again and then change to body quilt by default these are turned off consumed bodies and consumed quilts so i click okay at this point we only have one body listed in the model but once again if i go back to my tree filters and then go to body quilt i can have both consumed bodies and consumed quilts appear in the design tree as well let's take a look at a ui enhancement in assembly mode let's say i go to assemble a component let me grab the turret okay so i want to assemble this turret in here and let me just start positioning it into place a little bit the way that i want it to be again this is the same as in previous versions but you'll notice that the display of the dashboard has been updated so we can see that it's a little more prominent in terms of what the different icons mean because they have text explaining them here we have our connection type current constraint listed here we can see that for our component display it tells us what the icons mean for displaying them in the same window or a separate window and that way it's a little easier to understand where you'll also see a difference is the status so right now tells us that we have no constraints let me grab some geometry so for example i'll grab that cylindrical surface and this cylindrical surface so now it tells us that we are partially constrained let me select a flat surface might be easier if i pick the other one from this window and right now it says oh wait the constraints are invalid for some reason it wanted to give a normal constraint let's try a coincidence constraint and now we are fully constrained using assumptions if i uncheck the allow assumptions tells us once again that we are partially constrained and again if i try to give an impossible constraint like hey let's grab these two surfaces and make them coincident you can see that it promptly tells us that the constraints are invalid hey let's delete that one out of there let's turn allow assumptions back on and so now we are fully constrained using assumptions and now that we are fully constrained using assumptions let's hit the check mark so again just a little bit more information in terms of your constraint status and also an updated dashboard to make it easier to understand let's take a look at some different config options i will go to file options and again now there is an additional options command because you have the ability to manage ui customization right from a single dialog box let's cancel out of here and go back to file options options and so for some of the different options let me go to configuration editor i will hit the find button and let's search for 3d underscore datum and then click on find now so if i make this dialog box a little bit bigger you can see that we have two new options 3d datum display fill set to show or hide for the 3d datum's transparent fill also we have the 3d datum planes transparency control where you can set a value for the transparency percentage so those two options are new let me change in here to let's look up a different one enable legacy so we have enabled legacy datum planes and this one enables the legacy look and feel for datum planes default value is no but you could change that to yes if you're attached to the old way that they looked also if i look up csis we now have the csis color rgb which you can change between yes or no for the red green blue display of the coordinate systems for those different options as i mentioned earlier for things like your constraint display or dimension display if they don't have a config.pro option when you change those settings they are stored in your creole parametric customization.ui file automatically let's close actually let me stay in here because i want to show you that there are a few options now for better control of multiple monitors so here we have primary monitor and you can use this to control the number of the display to treat as the primary monitor on which to launch creo overriding the setting in use on the desktop another one that we have let me search on the term dpi for a couple of the new options there's one called dpi scale the custom display scaling size to be used to scale gui elements and controls overriding the setting in use on the dashboard also another one is high dpi text enabled that is another new option and another option that is related to your use of multiple monitors there's a hidden config.pro option it's called text underscore height underscore factor you could use that as well if for example you might have some vision issues if you want to make the text bigger in the graphics area that config.pro option will enable you to do that so there you have it a number of enhancements to the user interface and user experience in creole parametric 8.0 i hope you enjoyed this video for more information please visit www.creowinshill.com if you learned something from this video please give it a thumbs up and if you like this video please click the subscribe button and ring the bell to be informed when new videos are uploaded thank you very much

Channel: Creo Parametric

Views: 3,224

Keywords: creo parametric, ptc creo, creo ptc, creo parametric tutorial, creo parametric 6.0, creo parametric 6.0 tutorial, creo parametric 7.0, creo parametric 7.0 tutorial, creo 8, creo parametric 8.0, creo parametric 8

Id: U2ysaj8Pvd4

Length: 22min 34sec (1354 seconds)

Published: Wed Apr 28 2021