(3/31/2013 – The post below was written in 2010 and since that time Logopress has put in place something to automatically warn the user about splines, ellipses and parabolas if he or she forgets to do what is recommended in the post below. See related post dated 3/31/2013 named “Logopress3 warning regarding “nasty” sketch elements“)
Typically (almost always actually) we want to avoid using splines in our die designs. Just as most CAM software systems do not like working with these complex entities (and some won’t, period) sometimes CAD doesn’t like it either so we really must avoid using them in our Logopress3 strip layouts. Make sure there aren’t any splines in the flat blank of your Reference part and that way you won’t have any in your strip layout or in your wire EDM geometry such as punches, die blocks, etc.
It is a good practice to always check your flat blank at the end of the Reference Part if you think there is any chance that there may be splines in it. If you have already finished your Reference part, along with the last station mark for the flat part, roll back just before it this last station mark. Then, click a face of your flat part and start a new sketch on it. (If this flat face of your model is made up of multiple faces because, for example, an unbending caused a the main face to be split at one of the unbendings, then you should select each of these flat faces until the entire flat blank is highlighted.) Then use the SolidWorks Convert Entities command to convert all the entities around the perimeter of the flat blank. Now we want to see if these are all good entities or not, so we’ll use the Logopress3 command found with the other Logopress3 Sketch Tools called “Convert splines into segments and arcs”. A dialog box will come up in the Property Manager with a suggested conversion tolerance, simply accept what is already in this box by checking Okay. If there are no splines in the converted entities within this sketch, then the sketch will still be black since every segment will still have its On Edge relation that it automatically got from the Convert Entities command. If there were splines, you now have some blue, underdefined entities because these splines have now been converted by Logopress3are into either line segments or arcs.
Now you can either work with this existing sketch to fully define the new lines and arcs and make it nice, tangent geometry, or you can simply save this sketch and close it, understanding now what geometry on the flat blank needs to be “repaired” to eliminate the spline areas on it. For example, if you simply have an inside radius and an outside radius that showed up as being blue (spines that were converted to lines and arcs) it could be as simple as doing a delete face on the solid body blank in the corresponding inside and outside corners and then adding fillets that correspond to what is supposed to be there. Of course these new fillets will be comprised of arcs rather than splines.
You may feel it would be easier to work with the new sketch that was converted and use this new sketch to create your flat blank by fully defining all of this geometry and of course eliminating the splines. If this is the case, then simply fully define all of the entities in this new sketch or create new geometry as needed in this new sketch, deleting the geometry you don’t want to use (or making it construction geometry) and then you can extrude this sketch, being careful not to “merge” it with the first “bad” flat blank. Do a Delete Body on the original flat blank solid body to get rid of it. This method of creating a new sketch and new solid body is particularly a good idea if your flat blank had a lot of bad geometry (splines) in it or if it had one or more split faces due to unbendings and you would prefer to work with a cleaner blank.
(07/26/2010 – I would like to reinforce the fact that this method mentioned in the paragraph above is definitely the cleanest and most foolproof way of handling the flat blank solid that you have in your file just before the last station mark is created. Part of the reason for this is because even though the entities converted into a sketch may all show that they are not splines, it is possible that some dirty geometry still exists on the edge thickness of the solid body. By starting fresh with a new sketch that has no splines that you will be doing a BaseExtrude from, you are guaranteed a good, clean sketch. If this flat blank solid is left dirty, you may end up having problems later including, but not limited to, trying to use the Join command later to create a single solid body for the strip.)
After finalizing the blank, “audit” this blank by doing another sketch on it and converting the entities and using the Logopress3 “Convert splines into segments and arcs” again to check and make sure you have all black geometry. The second audit you should do after this first one is to right click on an edge of the flat blank and Select Tangency since of course we’d typically like to use good, clean geometry made up of fully defined tangent lines and arcs. If it is not important if you have tangent geometry for whatever reason, or if it is okay if some arcs are missing, then of course you can skip this audit.
Once you know that you now have a good flat blank, roll to the end of the tree, past the last Station Mark and then to a Ctrl+Q in order to rebuild this last station mark. If you have already started your annex part and your strip, then switch to either the Annex part or the strip assembly and use the command on the Logopress3 pull down menu called “Update the Annex part used in the strip”. When it asks you if you want to rebuild the Reference part, it is a good idea to answer yes, even though you may have just done a Ctrl+Q while in the Reference part. This assures that the body files will get updated. If you already have punches in the strip assembly, then the sketches will now have dangling entities in them and you can either repair them or delete these punches and remake them.
-IMPORTANT-1- info for LP3 users
