What's New in Creo 8.0

in creo parametric 8.0 you have enhanced control  over the appearance of dimensions in sketcher   use the toggle button underneath the show options   to turn background display on  off during the sketches session in addition you can fully configure the dimension  background appearance in the options menu color   and transparency can be set individually  for sketcher and 3d model dimensions with   full flexibility to define different dimension  background settings for sketcher and 3d modes   in addition sketcher dimension display is enhanced  and provides an ability to control the display of   weak dimensions which can be turned on off  during a sketcher session from the show menu the sketcher environment also provides  a more vivid dimension display   during the selection and pre-selection workflows  it also presents a modernized dimension dragger   so it is easier to see grab and drag previously  for some backgrounds and model colors it was   difficult to discover and interact with dimensions  this enhancement offers a better discoverability   and visibility of sketch dimensions and an easier  selection of dimension draggers for modifications in crear parametric 8.0 you have additional  options to control the default size of a datum   plane upon creation this can help to avoid  situations where large datum planes might   clutter the graphical model presentation more  than necessary you can choose between three   behaviors controlling the default datum size  the default behavior is unchanged to previous   versions where the datum plane default size is  automatically calculated to fit the model outline   if you change the value of the new  configuration option datum display default   from model outline to pre-configured size  new datum planes are created with height   and width dimensions as specified in the  additional configuration options listed here reviewing the details in the display tab you will  find the use display reference option unchecked   and the width and height dimension fields  pre-filled with the pre-configured user-defined   values for datum points as placement reference  the datum plane will be centered at that point   and parametrically follow positional  changes of the placement reference point an advanced third logic is offered when you  set the value of the new configuration option   datum display default to reference size this uses  the outline of the first placement reference to   define the initial datum plane size in that case  the used display reference option on the display   tab is checked and the display reference field is  automatically set to the first placement reference   note that you can also check use display reference   but remove the display reference from the  collector the system then refers back to the   entire model as reference and calculates the  datum plane size based on the model outline additional flexibility is provided through two new  behaviors of the use display reference checkbox   and display reference collector when the selected  display reference is of type vertex or datum point   in this case the display reference  point or vertex will determine the   center of the datum plane and you  can define the size in two ways you can check use display reference  in which case the datum plane width   and height dimensions are taken  from the pre-configured values uncheck use display reference in  which case you can manually define   the datum plane size by entering values into the  width and height collectors in the datum plane ui   if you want to recenter the datum plane during  definition you can quickly check and uncheck   the use display reference checkbox overall these  options provide you with increased flexibility   to tailor the datum creation workflows  to your needs helping you to optimize   design visibility with fewer repetitive  manual adjustments to datum plane sizes when creating a curve through points on  surface you can now create a geodesic curve   which will represent the shortest distance  on surface between the two selected points in this example we are referencing  the surfaces of the complete part as you see when changing the point location or the  geometry shape the geodesic algorithm will find   another path for the shortest  distance and update the curve in creo parametric 8.0 the flat wall feature is  enhanced to support the creation of multiple walls   at the same time you can select several  linear edges as placement edges for the   wall feature this creates a wall on each of the  placement edges based on the same wall definition   parameters share a common value for all  walls a change in the wall height bend radius   or bend angle is automatically propagated to all  walls created within the same flat wall feature   dimensions and draggers are shown for a single  wall only click on a wall preview geometry   to relocate the contextual dragger placement  to the selected multi-wall segment this   allows you to edit dimensions in the most  convenient location in the graphics area when you edit the underlying sketch it will  be edited as a 3d section which can only   be applied to a single placement edge as in  previous screen parametric versions convert   the 3d section to a 2d section to replicate  its placement on multiple placement edges   you can also open it to the sketch file  from disk depending on the way the sketch   geometry is defined you can have the  wall reference the endpoints of the   attachment edge and adjust to the edge length  or reference the wall midpoint and be centered again when you edit the bend relief definition it  will automatically be applied to the other walls you can select multiple adjacent straight edges  as placement references for the flat wall feature   the feature will then detect corners and  provide optimized default settings for   the corner treatment options outer corners are  typically created by default without a corner seam   for inner corners a default setting of create with  seam is preferable and used this automatically   avoids overlapping geometry in concave  wall-to-wall situations as illustrated here mitre support is also introduced in the flat wall  feature this applies to situations involving three   bend corners when you check add miter cuts  creo automatically trims overlapping walls   attached to bends meeting at three bend corner  and then creates a cut various options are   provided to control the gap width and position in  addition new three bend corner reliefs are created   the new three band corner relief types  within the flat wall feature include tangent   open closed and rip note that the miter option  is also available when the three-bend corner   involves already existing neighbor walls this  enhancement enables faster sheet metal design   with a fewer number of flat wall features and   aligns workflows and provided options  between the flat wall and flange feature creo parametric 8.0 offers a new  whole feature workflow option   that allows you to create multiple  holes in a single hole feature   the placement type of the whole feature can be  set to sketched it then takes placement locations   based on an internal or external sketch in the  workflow shown here we are for example creating an   internal sketch with a hexagon that will be  used to determine the hole placement locations   by default they are derived from  the end points of straight solid   lines in the sketch construction lines in the  sketch are ignored which can help you to control   which geometry should be used and interpreted  for the placement locations calculation   for external sketches the object action  workflow is supported after a sketch is   selected the whole feature appears as an eligible  command in the context sensitive mini toolbar   the locations of the hole can be defined  based on individual sketch points end points   and midpoints of straight sketch lines this new functionality is supported  for simple as well as standard holes the whole nodes are also available for  multi-hole features reference pattern   functionality is supported and it interprets the  multi-hole feature analogous to a base pattern   this is also indicated by the pattern  modifier on the whole feature icon the number of whole instances contained in  the whole feature is also used to call out   the number of holes in the whole node pattern  callout a straight pattern of multi-hole   features calculates the sum of all holes and  calls that number out in a single whole node   a pattern of grouped multi-hole features  creates a whole node for each group previously holes could only be created by  individual features and could not be created   directly based on sketches the workflow  required multiple features and included   an external sketch and patterned features  this enhancement offers improved productivity   through a faster and easier creation of multiple  holes in the part and assembly design workflows in creo parametric 8.0 there's broaden support  for the option to create holes in a lightweight   representation this option is now available  for all types of the whole feature in the   cryoparametric part modeling environment including  the standard holes and the drilled and sketched   simple holes that previously did not offer the  lightweight representation option no matter which   hole type you can now benefit from the lightweight  representation of holes to speed up regeneration   when working on a design that contains a big  number of holes such as large hole patterns   switch to the lightweight hole representation  by pressing lightweight representation in the   whole feature dashboard ui or from the right  mouse menu when selecting a whole feature   in the model tree the lightweight representation  is also propagated to dependent holes created   when patterning or mirroring hole features full  lightweight representation support for holes is   now also available in other creo part modeling  environments such as inside sheet metal and ecad in creo parametric 8.0 you have more flexibility  when defining threaded holes in both part and   assembly mode the whole feature provides enriched  threat handling options for thread length and   intersection control you now have more thread  depth options including through thread blind   and to selected reference giving you more  flexibility to control the thread length this is helpful when the drill depth  is geometry dependent as you can now   choose the through thread option when  you drill to a geometric reference   it is also beneficial if you want the thread  length to be driven by other geometry in the model   as illustrated here where the thread length is  defined to align with the depth of the slot shaped   cutout let's have a look at a few more examples  defining hole features in the assembly mode in the first example the drill depth is  defined as blind with a depth dimension of 45   the thread is defined as a through thread in this situation the  true thread is not trimmed and   its length corresponds to  the drill depth dimension in the second example a surface is  selected as an ob2 reference for the thread   in this case the thread surface is  trimmed by the reference surface geometry the same applies to the third example  here the same surface is selected as an   ob2 reference for the drill depth definition  and the thread is defined as through thread   this enhancement in creo parametric 8.0  allows faster and easier definition of   holes containing threads of geometry dependent  length and eliminates the previous need to   explicitly measure the required thread length  as input for variable thread length dimensions the whole feature in cryo parametric 8.0 is  enhanced for npt and ptf and iso 7 standard holes   it now allows you to create a straight  drilled hole in combination with a tap   tapered hole section the depth configuration  for the straight drilled hole section include   the options to drill to specify depth value  to drill to intersect with all surfaces to   drill up to a selected reference to drill  to next surface or through until a selected   surface which are options only offered in  all features that cut a single body which   is not the case the video here and finally  the option to not add a straight section   this last option represents the same  geometry as created by previous creo   parametric versions the new tapered tip checkbox  also provides additional geometric shape options   and allows you to toggle between whole geometry  that includes or excludes the taper tip surface   when you set the taper tip angle to 180 degrees  you can achieve a step function type change in   the whole diameter when the tapered tip checkbox  is not selected the straight drill diameter is   automatically calculated based on the tapered  hole size and the tapered section depth the   whole charts so the dot hole files are updated  to drive thread depth and straight drill diameter previously the creation of the tapered and  straight sections of tapped tapered holes   required the definition of multiple features  users often had to create a group of features   within a user-defined feature definition to  facilitate the whole creation for these situations   this enhancement improves  productivity and standard compliance   during the creation of tap tape at holes  in the path and assembly design workflows in creo parametric 8.0 the transparency control  workflow in interface has been improved based on   feedback received from our users no longer only  available in the view tab you can now access the   transparency control from the in graphics toolbar  the prior b rep filter has been separated into   their own filters one for solid bodies and one  for quilts this will allow you better control on   enabling transparency on your desired geometry for  components or solid bodies you can easily select   them in the graphics window and through the mini  toolbar make them transparent you can select them   again through the same process to turn off the  transparency once set as transparent you'll be   able to control the transparency value in display  through the transparency control settings having   said a few components as transparent you can  easily change the value of transparency from the   default fifty percent to let's say 75 or simply  use the corresponding slider the display updates   immediately you can now toggle the transparency  on and off to see it update on the screen   for surfaces quilts and tessellated geometry  the transparency is immediately controlled by   the transparency control settings by default  the transparency is set to a value of zero   however you can adjust that to see  the corresponding geometry update this   enhancement will allow you to quickly control the  transparency display of different components or   types of geometry without having to set a defined  appearance or appearance state it will provide   you an improved user experience when working  with different geometry representation types   creo parametric a.o features new sketching tools  for your drawings that can boost your productivity   this demo shows a workflow for  maintaining legacy imported drawings   without its model however the tools can be  also used for model views in the same way   first you will find that the new snapping  guides were added to the new sketch ribbon   these options let you decide what snapping types  will be offered as you sketch your geometry   as i move the cursor along  the geometry when sketching   the cursor will be snapping to other entities  based on the selected snapping guides   in the case that you've sketched an entity but  forget to create it as a construction you can   quickly toggle it between solid and construction  modes with this new shortcut menu option   you can also set the construction mode up front  and create any shape with the construction lines dragging behavior of sketched entities was  also updated so as you select your entities   and move them away to a new location you will  observe that you get representation for both   the old and new placements as well as on-the-fly  dimensions and set of reference control tools   for precise definition in this case i can  use the new toolbar define the reference for   the sketching starting point and input  the exact dimensions for the sketched shape the new tools also support mirroring  so you can quickly mirror your sketch   and avoid the double work many of the  new tools have several definition modes   for example in this case the slot actually needs  to be rounded at the sides so i can pick the   relevant arc sketch type pick the origin and the  two ends and quickly achieve the desired result as i continue my workflow of  updating this legacy drawing   i will add several reference lines to make sure  that i correctly adjust the bottom view as well but i need to add a reference for the geometry  to be related to i just need to hover over the   reference and it will be added to the  memory that will be reused as i sketch   note that after i hovered  over this vertical reference   line it is becoming easy for me to  drag this circle and make it tangent the same happens as i need  to align the second circle   as i hover over the referenced origin  i immediately get the relevant guides finally when i feel my sketching part is done   i can choose multiple sketch entities and decide  that they will define it to the draft view those views can be related to each other as  projection views be organized in the drawing   tree to show their relations to each other  and also be scaled at once to fit my drawing interaction with symbol palette was  improved with creo parametric 8.0   the new symbol palette now supports multiple  sheets so you can create a custom palette and   organize the company symbols in the best suitable  way after you find the symbol that you want you   can inspect it better with the new zoom to select  it command and right away place it in your drawing if a specific drawing contains a symbol that  you would like to include in your symbol palette   you can easily do so by picking it from the  screen and leveraging the new graphics toolbar commands when required you can remove  existing symbols from the palette   move symbols around to  organize the palette as needed   and save the result for the benefit of  other users who use the same symbol palette finally if you are the cad administrator and you  need to restrict users from editing the symbol   palette you can define the new config.pro option  restricted symbol palette with the value yes   and block the symbol palette  editing toolbar commands   creo parametric a.o introduces new advanced  contextual commands that can help you easily   place and edit symbol instances in both the model  and the drawings when placing a symbol you can   apply the repeat mode from the symbol ribbon pick  the symbol you want to place from the gallery   and place multiple instances in one go while  placing the symbol instances you can place them   with the automatic placement type or choose other  placement types from the contextual shortcut menu   if you have some symbols already placed that you  would like to leverage you can save some time and   quickly repeat them using the new repeat command  that is available in the contextual mini toolbar now that all of the symbol  instances in my example are placed   i can quickly customize them and  edit their properties as needed if i need to add the orientation and scaling of  this symbol i can update it from the contextual   ribbon properties or use the new contextual  transform command from the mini toolbar   once activated you can use the appeared draggers  to update the symbol to its new position or scale   finally if a new version for  my placed symbols was updated   i can pick one of the symbol instances choose the  new update symbol command from the shortcut menu   and all of the instances will be updated creo parametric 8.0 includes quite a number of  new model 3 capabilities you can for example   create custom groups in the design items folder  the display can also be controlled in the model 3   filter settings custom groups enable you to create  a custom structure to organize design items for   example by dragging bodies and quills into custom  groups this allows you to document your design   intent with more flexibility and freedom for  example to reflect functional areas in your design   you can create custom groups name and rename  them use dragging to reorder them and structure   them to freely manage quilts and bodies  according to their function in the design   to organize an existing design you can drag bodies  quilts annotation elements and material nodes   into or out of these groups in a custom  group when you right click the item and click   remove from custom group the item is  relocated to its original position   for example when you remove a body from a  custom group the body is relocated to the body's folder the presentation of bodies and quills in a  custom group includes contributing features to organize a design as you go you can set a  custom group as default the default custom groups   are marked with a star newly created items will  be automatically added to the default custom group in the illustrated example here the krilt  representing the parting surface to split   the housing body along with the new bodies  representing the top and bottom parts of the   housing are all automatically created  under the default custom group called split creo parametric 8.0 makes it easier to  organize the design and to allow design   engineers to document their design in a way  that others new to the design can quickly   grasp the evolution and functional grouping  of bodies quilts and other design items creo parametric 8.0 supports a design tree and  side-by-side trees you can split out the design   items folder into a separate design tree  this allows you to control scrolling and   visibility of features and design items  more independently and in the right context   to hide or show the design tree check  design tree in the model 3 options note   that the design tree remembers its expansion  state when you hide and then show it again you also have more options to tailor the tree  display to personal needs and preferences   secondary trees such as the design tree  or the layer tree can be dragged out and   stocked to various places on the border of the  graphics area or within the navigator panel you can also split the model tree into  two independent trees for example to   show a combination of the design tree and the  model tree or the model 3 and the layer tree when docked within the navigator panel the trees   share the same visibility control  and behavior in full screen mode when the design tree is docked to the border  outside the navigator panel its visibility can   be controlled separately from the visibility  of the model tree in the navigator panel   you can also display more  than two trees and for example   show the model 3 the design tree  and the layer tree at the same time   when displaying the design tree separately you  can enable simple search for it this allows   for example to search for a body or quilt with a  specific name within the body folder quilt folder   or custom groups in addition you have the option  to configure the design tree settings separately   this allows for different design tree filters or  design three columns when showing the design items   in this secondary tree note that you can also  turn on auto locate for the separate design tree   selecting geometry in the graphics will then  auto locate related features in the design tree   if they are contributing to quills or bodies in  parallel features will then also be auto-located   and highlighted in the model tree this provides  for a very fluent interaction with both trees at   the same time giving access to features in the  model tree following the regeneration sequence   and to bodies and quilts in the design items  tree where they can be organized in a custom structure the varied items table for flexible  components has been improved   each type in the varied items dialog  box indicates the number of line items   in that tab the heading of the dialog  box indicates the total number of lines when you select a line item in the table  the corresponding component and its features   are highlighted in the model  tree and in the graphics window this enhancement makes it easier to understand  the involved components and its features and   provides a clear overview of the applied varied  items for each tab in the varied items table we've added two new checks for model check in  creo 8.0 one check the body interference check   expands model check support for multi-body  workflows first introduced in creo 7.0   another check for weak sketcher dimensions  has been highly requested by creo users   both of these checks will report errors  warnings or just the check information in this model i have the main body in a cavity  that will cut a channel in the main body however   checking for body interferences i can see that  these two bodies do in fact interfere with one   another i can see that the cavity geometry  was not subtracted from the main body so   applying subtraction i can now see that the  bodies no longer interfere with one another   in the model check report i can also see that  there is a sketch that contains weak dimensions opening up that sketch i'll  make those dimensions strung   and then i can rerun the report  to see that the check now passes with these new checks creo users will have further  options to ensure their models are well designed   and follow company best practices

Channel: CADx

Views: 7,082

Keywords: what, what's, new, in, Creo, 8.0, part, drawing, ptc, parametric, creo 8, creo 8.0, creo8, creo8.0

Id: Orn4vWlRo4c

Length: 36min 25sec (2185 seconds)

Published: Fri Apr 23 2021