Creo Parametric - 5 Sketch Mode Tips and Tricks

to examine the sketcher Diagnostics tools I'm going to create an extrude with an internal sketch if I select a flat planar surface or datum plane that puts me immediately into sketch mode and let's change to our sketch orientation and I'm going to start off by importing a sketch and let's change the scale to 1 and I'm just gonna drop it right in the middle here and hit the check mark and right now I have my dimension and constraints display turned off just because it clutters up the screen in this situation in the ribbon you have a group of commands in the inspect group that provide different diagnostics tools and two of them are on by default shade closed loops and highlight open ends and highlight open ends you can see over here a little bit unfortunate I have a red model here but it highlights it in red where we have an opened end over there and we don't have a closed loop because this area is not shaded by the way if you want to turn those two buttons off by default you can do that by going to file options configuration editor and if you click the find button and then search on the word sketcher you can find there is sketcher highlight open ends and sketcher somewhere in here shade close loops again the default values for those are yes and you could change them to know if you want but I like having those options turned on so I'm going to cancel out of there and also we have this feature requirements button when you click on it it'll give you a list of requirements in whether you comply with them or not so it says that the section must contain geometric entities that's checked multiple loops must all be closed weird checked and it says not all open ends have been explicitly aligned and cannot have more than one open loop so let's go about fixing the problem and one tool that you can use for doing that is highlighting overlapping geometry right now it's highlighting over here indicating that I have overlapping geometry again when i zoom and I can see that we've got this a little bit of extra segment so I'm going to use squiggle trim or delete segment to get rid of that and we no longer have red highlighted therefore that open end I see some red highlighted down here at the bottom so here we have a gap inside of here I can use the corner tool and pick the two entities to extend them to one another and now you can tell that the loop the closed loop has been shaded as per this button over here and if we go to feature requirements we have two checks over here everything meets the requirements of this feature so now we can use the check mark from the right mouse button menu to get out of sketch mode and I can drag this to the desired depth that I want and hit the check mark and that way we've used our sketch or diagnostics tools in order to create our feature let's take a look at the replace command in sketch mode so I've got my part over here just a few different features and I decide that I want to change the shape of the protrusion so I'm going to edit definition if I go to the placement tab this also has an internal section I can click the edit button and let's go to our sketch view and I decide that hey you know what I don't want this to be a straight line I want to put an arc in there and so if I select that line and then hit the Delete key I get this worn that says wait this entity is referenced by other features do you want to continue what creo parametric has told me right now is that if I hit the yes button I'm going to get a regeneration failure and I'm not going to heed creo parametric warning in this case I'm gonna say yes I want to get rid of it we've got our openings highlighted let's throw in an arc and just gonna create in here about yay big I'm not really gonna care about the dimensions in here let's hit the check mark and hit the check mark to complete the feature and now we see that we have a notification that we have a regeneration failure and the round in the model tree is failing so let's undo this and I'm going to show you the proper way in order to make this change so let's select the protrusion edit definition go to the placement tab and click Edit to edit the internal sketch I'm gonna go back to my sketch for you and instead of deleting this entity because again if I try to do that I get the warning I'm going to heed the advice and say no I'm going to create my new entity let's create our arc oops going out of the wrong part of the target there we go and and I'm just eyeballing it and now I've got my new entity selected if you go to the operations overflow menu there is a replace command and just checking real quick see if you get it up it's also available in the mini toolbar and when I click on that right now I'm getting in Arizona oh wait incorrect choice must pick old entity so I like that little help there so you start with the old entity and then choose the replace command and then pick the new entity and everything is good now when I hit the check mark and the check mark for the extrude feature I don't get a regeneration failure because essentially the replace command will transfer all the children of the geometry that's created by the old entity with the new entity so transfers those parent-child relationships and helps you avoid having regeneration failures Here I am in sketch mode and I'm going to take advantage of what's called the palette the palette has a number of predefined shapes and by default the palette has four different tabs the first one is the polygons tab and has everything from a three-sided trying to make this a little bigger rearrange this in here 8 3 sided 220 sided polygons and from the profiles tab we have AC shape I shape L shape and a t-shape let's grab the C shape and I can drop it on the screen and you've got a drag handle for rotating this I'm gonna rotate it 90 degrees and also we have a button to change the scale and I'm going to change this scale to a value of 40 and we have a drag handle to change the drag location put position your mouse over it hold down the right mouse button and drag it to the point that you want to use as the drag location and then we can drag the figure where we want it to be and when we're happy we can hit the check mark you'll notice that the sketcher palette remains open so that you can place additional features in here besides the profiles tab you all to have a shapes tab and you can see that we have a couple different waves in here arc racetrack or angler racetrack rounded rectangle cross and oval and similar to the polygons tab we have the Stars tab with everything from a three tipped star to a 20 tipped star you'll notice in here I have an additional pallet tab and it's got three different figures in here and that's because I have a config dot profile that excuse me configure our profile option that points to a folder where I've stored s-e-c files if you go to file and then options I'm gonna go to configuration editor there is a config Pro option called sketcher palette path and I have it pointing to a folder on my computer you'll notice that that older is the same name as the tab that we have in the sketcher palette dialog box besides using this particular options there is another option I'm gonna click the find button and type in 2d and it's called 2d palette path it does the same exact thing as the sketcher palette path config dot Pro options you can use either or I believe even both of those options to add additional tabs to your sketcher palette so that you could quickly and easily reuse sketches in your model let's take a look at using both the sketcher grid and applying cross-hatching to a sketch I'm going to start out by creating a sketch by clicking the icon in the ribbon and before I pick my sketch plane I'm going to go to the properties tab and you'll notice that we have some great out text in here for add cross hatching and choosing the scale and the angle for some reason you're not allowed to define cross hatching before you make your sketch so I'm gonna select a plane to sketch on let's go into sketch mode and I'm going to change to my sketch view and first off let's turn on our grid that we can use I'm going to go to the setup drop-down menu and then display and here we have grid display you can also get to that from the display commands in the in graphics toolbar so let's turn on the grid display and reduce clutter let's turn off our datum plane visibility and if i zoom in you can see there faint gridlines on here if you go to the setup drop-down menu you can go to grid settings and you could either use a Cartesian grid or a polar grid let's start with a Cartesian grid and right now the spacing is dynamic in other words as you are creating your different entities it's going to adjust the grid appropriately for you but you could also change to a static grid and let's say I want a one by one grid also you could choose to change the origin to some other location if you wanted to and you can also rotate the grid by some angle but I'm going to leave it at a zero degree angle and sometimes when you're sketching it does become helpful to have a grid especially if you're trying to make a regular shaped figure and you already know the general proportions or dimensions that you want to use and also in addition to using this grid if you go to file options and then sketch her you can turn on the option for snap to grid and this corresponds to the config Pro option grid underscore snap and so I can turn that on and click the ok button I'm not gonna add it to my config dot profile and now when I go to create a line you'll notice that hopping around on the screen for the starting location wherever I move my mouse based on where that where the different grid point locations are in the model but let's delete this I'm going to also show you how to do a Cartesian grid so we go to set up grid settings and excuse me I'm and I wanted to show you how to do a polar grid and for the polar grid let's zoom in over here right now we have a radius of one fourth grid and we have angular angular interval of 30 degrees and also 12 grid lines you can change either or they're obviously tied to each other so for example if I change this to 10 well then they're going to be 36 degrees apart and if I change this to 45 I'm going to have 8 grid lines and so now I still have my grid snap turned on I could use this to create geometry and again make it out over here and it's snapping to the different locations and then close it off here that's good I'm going to hit the check mark and oops where did my sketch go there I have my sketch created now let's edit definition in order to turn on our cross hatching now if I go to sketch setup and the properties tab I have the ability to check the box to add cross hatching and here we have our scale based on how big I made this I'm gonna guess that I want this to be a little smaller and right now it's at a 45 degree angle let's hit the sketch button and go to our sketch for you just that we're looking right on it and now when I hit the check mark you can see that our sketch has hatching if we decide that we want to change it and just edit definition and go to sketch setup and go to the properties tab and then you can say hey you know instead of a 45-degree angle I could use this drop-down list to choose a different angle maybe I want to 60 degrees and maybe I want it to be even tighter cross hatching hit the sketch button hit the check mark to get out of sketch mode and there you see cross hatching applied to the sketch I hope you enjoyed this video for more information please visit www.hp.com/recycle please click the subscribe button to be informed when new videos are uploaded thank you very much

Channel: Creo Parametric

Views: 10,571

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Id: x6cEmj0YjEk

Length: 14min 47sec (887 seconds)

Published: Wed May 22 2019