ACCEPTED SOLUTION
Accepted Solutions
Thank you for providing the additional info and the image. The pinkish color you are referencing in the training guide is the color used to represent a closed sketch, regardless if there are constraints or not. See an example of a sketch with only one coincident constraint and weak dimensions. The filled in color is only for indicating a closed loop and does not indicate a fully dimensioned and constrained sketch.
My best guess for the discrepancy is one of two things (or both):
- Your company has set their own default colors for closed loop regions and the text. Older versions of Creo used the yellowish color instead of the pinkish color so it's possible that this was modified internally within your company. You can see this info in the "Options" menu found by clicking "file" in the top left.:
- You are using a different version of Creo Parametric. The course content you are using was updated for Creo 10.0 (and it is switching over to Creo 11 today). So some of the UI may look different, but you should be able to constrain the sketch the same.
Based on the image you provided, it seems as if you were able to match the dimensions and constraints of the image in the discussion slide. This leads me to believe, your company has a different customization than the default "out-of-the-box" Creo Parametric install. If you are noting differences like this, focus on the concepts and skills. In this example, if you are able to successfully recreate the sketch and apply appropriate dimensions and constraints, it seems as if you are doing things correctly.
One additional thing you could check is if your theme is different. In the "options" menu, if you are using the "light" theme then your shaded region will appear yellow. If this is the case, you could quickly change to "default" to see if the sketch you created more closely resembles what you were hoping to achieve. See the image below for how changing the them changed the sketch in the image I sent in the previous reply.
Hello,
The Custom color setting in the Theme happens if you choose a specific theme (Default, Light, Dark) but then further modify any of the individual colors. You can export these colors out (clicking the Export button at the bottom of the dialog) and then setting a config.pro option to point to this exported system colors file (syscol.scl). That will make it such that your colors are retained going forward. Your admin should be able to help you in this regard. Or search for how to do this in the PTC Knowledge base.
Regarding your additional questions:
1. I'm not sure why there is a difference in the constraint "glyph". I assume it's the same constraint but a different version of Creo (this might be a pretty old image from the course). When I re-created this sketch my point-on-entity constraint has a horizontal line like yours.
2 and 3 - I've duplicated your sketch:
If you look at both your sketch and my sketch you'll see that there is a weak dimension present on the left side (this is the light blue dimension that says 0.00 that is kind of hidden behind the parallel constraint).
So technically our sketches are not properly constrained. Or they are, but you're letting the system make a decision for you.
The weak dimension notwithstanding, if you cursor over the circular constraints it says "Constraint (Coincident Vertices)". If you select either of those constraints and click the Explain icon (expand the Constrain group and click Explain) the centers of both arcs highlight and the message window says, "Highlighted vertices coincide". If I delete those 2 constraints and apply the Coincident constraint to of the arcs to the vertical and horizontal reference I am able to get the same constraints as what are in the slide. There are 2 sets of these constraints because I made both arcs coincident on both references:
I just recreated the sketch from scratch and this time I got the constraint result like that of the slide image:
The truth is I don't have a good answer for why there are slightly different solutions here. It's very good that you're considering design intent here because these types of constraint differences can definitely influence the geometry outcome if you modify dimensions. In this particular case, however, I'm not sure the geometry result would change at all given the nature of this specific area of constraint.
I suggest reaching out to Technical Support for further questions like these. They will be able to help you better than me.
Regards,
Matt Huybrecht
Hello,
By default, Creo will add constraints and dimensions automatically to maintain a fully dimensioned, fully constrained sketch. The system has added that dimension because it has to add it in order to mathematically fully constrain it.
I think the best way for you to figure out why the system added that weak 0.00 dimension is to modify it and see how the sketch updates. For example, I've updated my value to 20, and you can see here what the result is:
There are other ways to constrain/dimension the sketch to remove that 0.00 dimension rather than using the Perpendicular constraint. Alternatively, if you click the Coincident constraint and select the 2 short diagonal lines the system tells you there is a conflict - the conflict occurs because the sketch is now OVER-constrained and you have to tell the system which thing to remove:
So if I now delete the 20 dimension, the system makes the 2 lines Coincident (or in this case, Collinear), and the dimension is no longer needed:
If you know you want both of those lines to always be the same length, then you can remove one of the 15 dimensions and use the Equal constraint to make both lines equal length. Thus, the length of both lines is now controlled by a single dimension:
The goal here is to dimension and constrain your sketches in such a way that the geometry updates predictably when you need to make changes.
Regarding the bold lines, it's probably one of a few different things:
1. I have Lines Anti-Aliasing enabled (File > Options > Options > Entity Display > Lines Anti-Aliasing).
2. My screen grabs are smaller than yours so I'm zoomed out of the model more. This makes the dimensions and constraints larger with respect to the actual sketch (they stay the same size regardless of zoom level) so my lines might appear thicker.
3. You can adjust sketcher geometry line thickness - I can't remember which Creo version they added this enhancement. Mine is set to the default but perhaps your admin changed it in your config.pro. The config option is sketcher_line_width (default value is 1.5), or you can change it in File > Options > Options > Core > Sketcher > Line thickness:
You're very welcome! You're thinking about this the right way. The dimensions and constraints you choose can greatly impact your geometry in terms of how it updates when you make changes.
Best practice is to NEVER leave any weak dimensions that the system auto-generates - YOU should be in control of your geometry because you know best how you want it to update. As you continue using Creo you'll pick up on how the system likes to snap constraints (incidentally, this is configurable). Making your sketches exaggerated and then using dimensions and constraints to refine them works well in helping you get what you want.
If you're ever interested in seeing how your sketch will update based on dimension changes, I suggest picking a dimension or dimensions in the sketch and clicking Modify. This will open a dialog box with the each dimension you select. Next to each dimension is a slider:
You can then drag the slider to dynamically increase/decrease the dimension value. This will give you insight into how the geometry will update as you dynamically change those dimensions.
Creo is crazy powerful, but as the saying goes, "With great power comes great responsibility".
Matt
