As you can see in the before and after pics below, the top picture has annoying looking white areas on some edges of the model. Here is the simple setting change to clean this up:
Go to SolidWorks System Options, Display/Selection, Anti-aliasing, and change the default “Anti-alias edges/sketches only” to “Full scene anti-aliasing”.
LP3 tips & tricks, SolidWorks tips & tricks
I’m embarrassed to say that I am guilty of not using this very simple tip very much myself over the years, and so I suspect there may be others like me that are overlooking this same thing.
Whether you are in SolidWorks or in Logopress3, when you are not sure how to do something, or if you just want a refresher to make sure you understand all of the benefits and options of a certain command, the quickest way to find help is to simply click on the question mark in the upper right hand corner of the property manager.
LP3 tips & tricks, SolidWorks tips & tricks
Logopress has added an extremely helpful warning regarding Splines, Ellipses & Parabolas (AKA nasties). This new warning is displayed when validating the property manager of the Annex part if it finds any nasties in the Blank section sketch. (When creating the Annex part, Logopress3 automatically creates the Blank section sketch and this is the sketch that is used to automatically or semi-automatically create the internal punches and the external punches. It is practically always very important for multiple reasons that this sketch does not contain nasties.)
Here’s how it works:
When unbent it looks like this
When you select Part preparation before strip starting to create your Annex part, and after you select your options in the Part preparation property manager and validate, you will see this warning dialog pop up:
It will highlight the nasties that are in the Blank section sketch and prompt you as shown and you should definitely answer Yes. At this point Logopress3 will create a new sketch at the bottom of the tree that shows the nasties like this:
This is extremely helpful because it shows you all of the areas in your Reference part flat blank that need to be cleaned up. It is important to note that you should not clean them up here in the Annex part, but rather in the Reference part. Open your Reference part and roll back to just above the flat blank station mark as shown here:
Select the Delete face command in SolidWorks (Insert, Face, Delete…) and highlight the area shown below (always be sure to select the option Delete and Patch when working with a solid body) and validate to remove this nasty area in the part. Doing so causes it to be absorbed by the true radius to the right of this nasty area.
At this point you should roll to the end of the tree and do a CTRL+Q (SolidWorks forced rebuild) which causes the Logopress3 body files to be recreated. Now open the Annex part, then select the Logopress3 command from the pull down menu called “Update the stations of the Annex part used in the strip”. This will import the newly created body files and cause the Blank section sketch to get recreated based on the new, clean flat blank. Note that as you can see in the picture below the sketch at the bottom of the tree that Logopress3 automatically created called “Sketch showing the splines on the flat blank” now has dangling relations in it. You no longer need this sketch so you can simply delete it.
-IMPORTANT-1- info for LP3 users
In AutoCAD there was such a thing as a Construction Line. In a sketch that is in a SolidWorks part file, a sketch entity (lines and circles are the most common ones) with a centerline linetype are always considered construction geometry. So you may see or hear some reference to a centerline as a construction line, or as construction geometry.
From the SolidWorks help file:
“You can convert sketch entities in a sketch or drawing to construction geometry. Construction geometry is used only to assist in creating the sketch entities and geometry that are ultimately incorporated into the part. Construction geometry is ignored when the sketch is used to create a feature. Construction geometry uses the same line style as centerlines.”
When you want a new construction line to use as construction geometry, it can be drawn as a construction line right off the bat because there is a separate command for a construction line. That command is simply called Centerline.
When you want a new piece of construction geometry that is a circle (this is not nearly as common as wanting a new construction line), this is not quite as simple as drawing a new construction line because there is no separate command for drawing a construction circle as their is for drawing a construction line. The new circle needs to be drawn on the screen first and then there is a check box in the property manager to change the circle to construction geometry.
If you have regular lines or circles (or other sketch entities) that you wish to turn into construction geometry, you can select the entity with a normal left click (or select multiple entities by holding the Shift or Ctrl keys as you select) and then on the shortcut menu that pops up you can select the icon to change to construction geometry. But it is quicker in the case of lines and circles to just draw this geometry right off the bat as construction geometry.
- It is common to draw straight construction lines right off the bat as opposed to drawing a line first and then checking the “For construction” option in the property manager.
- It is common to be working in a new sketch and convert entities from another sketch into the current sketch. (This produces an on-edge relation.) These newly converted entities could be “regular” geometry or if you wish they could also be converted into construction geometry.
- It is common to be working in a new sketch and convert an edge or edges from a solid body edge (including tangent edges in the case of dimensioning a form punch for example) into the current sketch. (This also produces an on-edge relation.)
SolidWorks tips & tricks
The names for Logopress3 Station Marks are automatically generated by Logopress3 as they are inserted. The name that is automatically generated for the very first Station Mark is 010 STATION MARK, the second one that is inserted gets named 020 STATION MARK, etc.
We strongly suggest not to change the number portion of the Station Mark, unless you are changing it to a different 3 character number for good reason. When you insert a Station Mark in the tree that falls somewhere between the 010 Station Mark and the 020 Station Mark, it gets named 015 STATION MARK. A Station Mark added between 010 and 015 automatically gives you 017 Station Mark, etc.
While we strongly advise you to keep the first 3 characters of the Station Mark names for organizational/sorting purposes, we also strongly advise you to name your Station Marks. We sometimes see example strip layouts with the default Station Mark names and wonder how a person keeps organized by not changing the “STATION MARK” portion of the name to something more logical like “010 FINAL FORM DOWN”, and 020 PREFORM DOWN, etc. When you are first creating the strip, if there aren’t many Station Marks you may not see a need, but if someone opens the strip layout other than you, or you open it months from now, you will probably wish you had named them to something logical. It doesn’t take long to do and you, or someone working on your design will be happy you did.
LP3 tips & tricks