A Knowledgebase for all Die Designers…

As long as I’m on a roll this month talking about balloons and how they work with the Logopress3 BOM, I figured I might as well show you a few details about the Logopress3 BOM and describe them. As mentioned below, there are many options making it very flexible and useful.

In the picture above, the first thing you see is the template being used at the current time. If you’d like to use a different template, simply switch it at any time.
The second thing you see is the list of parts, some of which are tagged (checked) to be in the bom and some of which are unchecked (the unchecked ones are not visible in the picture above). This list also shows you whether the part is locked or not, so it is shown as unchecked, checked or locked. This list also shows you, with both a graphical icon in the second column and a letter in the third column, which sub assembly this detail is in, be that the bottom, middle or lower.
The third thing you’ll notice is a button with a 1.2 on it and that button opens up the Number settings dialog, which is the one mentioned in the previous post that give you the options for balloon numbers, including which of the five organization methods you’d like to use.
The fourth thing is the padlock icon, and depending on which item or items in the list are highlighted may be available or grayed out if they are already locked.
The fifth thing in the list is a very nice feature – “Families of components to include/exclude”. In this picture above, you can see we have chosen to exclude the socket head cap screws from the BOM but have chosen to include the socket head stripper bolts and the pad retainers…
Finally, the last thing you see in the Logopress3 BOM property manager screen shot above is the “Add Custom Properties” list. This is an awesome feature that we’ve added quite recently that allows you to automatically populate every single part file in your assembly with custom properties of your choosing in the list in a matter of a couple seconds. The files don’t get opened, they simply get populated with the data. Of course you want your sheet formats to include placeholders for these custom properties so that the title blocks are completely and automatically filled out with absolutely NO user intervention other than filling in these spots in this “Add Custom Properties” area shown above!

In the case of standard components, as you can see in the picture below, these are represented in the second column with a picture of the component rather than an icon showing which sub assemly they are located in as is the case with “plates” that are inserted in the die in the screen shot above. But as you can see below, in the case of a standard component where some are located in the bottom sub assembly and some are located in the middle sub assembly, (the Lamina bushings and the 1/2″ long button head cap screws) they are listed in both as is represented by the MB.

If you were wondering what the H, M, and B stood for in the column heading above, of course the M is Middle and B is Bottom – the H is Highest, which of course is the punch sub assembly.
Finally, some might be curious if the part numbers happen automatically as the part is inserted into the die – the answer is YES!

LP3 How-To's for users

First of all, to get something straight and so that we are on the same page, when we talk about ballooning we are also talking about the BOM (bill of materials). The two are linked together and perhaps this is obvious, but it is worthwhile noting.

I’d like to point out just a few of the options related to the Logopress3 BOM and ballooning since they provide some nice enhancements over the standard SolidWorks BOM and balloons. There are a great deal of options in the Logopress3 BOM which provide the tool designer with a great deal of flexibility and the best way to learn about them is through the excellent Logopress3 help file. You will find a Bill of Materials section at the end of the Logopress3 help file that is absolutely loaded with just about every option imaginable or necessary to the die designer.

But it is worthwhile to point out just a few of the ballooning options to give you a flavor of what you can find if you dig deeper. Don’t let all of the options below scare you! Again, they bring flexibility and once youv’e used it on a design and determined the way that suits your company or your customer best, you know how to use it on the next design.

The picture below shows that Logopress3 has five main options for balloon organization.

Below we can see the first and most basic balloon organization method, “Global numbering”.

The picture above also shows a drop down box showing the three options that are common options regardless of which of the five balloon organization methods are chosen.

The picture below shows the “Global numbering according to the Balloons positioning order” method along with the options for sorting direction. 

It is the fifth option below which is my personal favorite because it provides the most information possible, “Split numbering for lower, middle, upper parts, and standard components”.

With this fifth option shown directly above and with the other two that are not shown, you might get the impression from the pictures above and from the help file that you can’t sort the balloons within each of the “groups” (in the picture above, I am calling the “groups” the upper, middle and lower sub assemblies, and standard components).
But in fact you CAN!

You can easily manipulate the software to do so through a combination of the above pictures along with the Logopress3 locking feature shown here in the help file…

…and as shown here in this screenshot:

But if all you want is to have the balloons sorted in order and not pay attention to where they are in relation to the lower, middle and upper sub assemblies and the standard components, then use “Global numbering according to the Balloons positioning order”. Instructions for its use are shown below – this is a screenshot directly from the help file:

LP3 How-To's for users

For those of us that were accustomed to using software in the past that automatically sorted the balloons so that they were in numerical order in the drawings, it was a real disappointment losing this ability when switching to 3D. With dozens and dozens of balloons on one sheet, or even over a hundred, it can be like playing “Where’s Waldo” when we searched for them.

This is not a problem with Logopress3 since Logopress3 has some very nice and very flexible balloon sorting tools built into the Logopress3 Bill of Materials (BOM). This sorting can be done in regular balloons, but used in conjunction with a split balloon, and also with using part numbers for parts rather than the names of parts or the description of the parts, this can bring a great deal of order on the manufacturing floor.

How much would the guys in the CAM department like it, and how much more efficient would it be to have the files all in order in a folder so that they don’t have to search for them – like this:

So if you are going to use a part number for the filename rather than a descriptive name for the filename, my suggestion to you would be to use split balloons. This way this is you can sort them and have them in order. This ordering of the balloons would be managed by the contents in the top half of the balloon using an automated Logopress3 custom property named “NumberNomenc”. The bottom half would contain the part #, minus the project number, which is, as you’ll see in the picture below, the “Comment” custom property.

It’s much simpler than it sounds. Below are instructions on how to do it (sorry if some of it is redundant):
The top of the split balloon is what we will informally call the “Detail” number. We call it “Detail” number because SolidWorks does not use this word “Detail” number. SolidWorks uses the word “Item” number and the “Item” number is NOT what we will be using here. In fact, this “Detail” number will actually be a Logopress3 custom property named “NumberNomenc” and Logopress3 uses this custom property for sorting of balloons.

The bottom of the split balloon will show the Logopress3 custom property named “Comment”. This Logopress3 custom property named “Comment” gets combined with the Logopress3 custom property named “ProjName” and this is what becomes the filename, with the SolidWorks extension of course. Note that Logopress3 has recently made available the option to have the project name (ProjName) either before or after the part name or number (Comment). So the file name could become ProjName+Comment.sldprt or Comment+Projname.sldprt. Below is a picture of the Logopress3 Tool Structure property manager and this picture shows you when the “Comment” custom property is chosen by the user, as well as the “Description” custom property, which will end up in the BOM and in the title blocks of detail drawings.

Below is a screenshot of what the custom properties look like within the part file for this part number 006 that we inserted:

Start by inserting your BOM using the Logopress3 BOM and change settings within the Logopress3 BOM as desired. Then insert your balloons using SolidWorks Auto-ballooning functionality or you can insert them manually. If the balloons are already there, just highlight them all and then go to the property manager and set to split balloons and set the top of the balloon to custom property “NumberNomenc” because it is this custom property that Logopress3 will use for sorting the balloons. This “NumberNomenc” is what we will loosely call the “Detail” number. Again, this is different from the SolidWorks “Item” number. The bottom of the split balloon will be set to the Logopress3 custom property “Comment” and, as mentioned earlier, this is equal to the file name minus the project number and minus the extension of course.

If you only want a single balloon and you want this to contain the part number, which is the “Comment” (file name minus project number and minus extension) custom property, this is no problem. You can simply set this single balloon to be the custom property “Comment”. But note that if you do this only, you will NOT be able to sort the balloons in numerical order using Logopress3 because it uses the NumberNomenc” custom property to do that and NOT the “Comment” custom property.

LP3 How-To's for users

It is very surprising to me that more tool and die companies don’t work with part numbers as the file name as opposed to the name of the part (the description, really) as the file name. I think the reason they don’t is because when most companies start out using 3D CAD, they start by naming the file “Die Block.sldprt” because that just seems more natural than just a number, and that is why some of them still do it this way years later. Also, it is intimidating (at first) to look at a folder full of numbers as file names as opposed to a folder full of “names” as file names. But once you are used to this, it is intimidating to look at a folder full of names as opposed to orderly numbers.

Of course the rest of the world works with part numbers typically rather than names. For example: If you buy anything at all for your home or car or whatever, and you need to order a new part, you look at the diagram of parts and most of the time you look at the balloon that is pointing to the component you need and look to see that this balloon is pointing to part number 12345 or whatever and you order a 12345. Or perhaps there is simply a part number being called out with a leader.

I believe there are two really significant benefits to using a part number (such as 17033-006 where 10733- is the project number or job number and 006 is the part number) for the file name rather than a descriptive name:
Benefit #1:
Many if not most dies cannot be designed fast enough for managment - they want to get steel on the floor and start cutting… So there is typically a problem because the BOM is not done yet and so you don’t know what the detail number is going to be, assuming you want your balloons in the correct order, etc, but of course you’d like the steel you order to be identified in some way. Using a part number allows you to order material based on the job # and part # combination and this part number is determined the minute before the designer puts the part into the assembly. So even if the part isn’t finished yet, you know what size it is and what kind of material, etc…
Benefit #2:
Back when we were using 2D, it was a major pain to have each detail on it’s own drawing – this often meant having each detail drawing as its own file. But today, with 3D and in particular with Logopress3, it is far easier to have each detail on its own drawing and being its own file. In addition, with all parametric modelers, including SolidWorks, each part file is its own separate file and these separate files go into an assembly. So it is much easier to locate these files in a folder or directory if they are in some sort of order. Giving the files a part number rather than a descriptive name brings this order to Windows Explorer and this way the CNC CAM operators and the WEDM operators and everyone else can find the files much more easily, as you can see from the picture below.

Benefit #3:
Having sheet numbers is just not necessary anymore in most cases, unless you need to keep doing it because “We’ve always done it that way“. We are creatures of habit, and sometimes this is the reason we do still do things like we did years ago. Instead of sheet numbers, many folks just use the part number of the part as the “sheet number”, so to speak. It’s not actually called the sheet number because you don’t look for sheet 22, you look for part number XYZ…

I would encourage you to look at the possible benefits of using part numbers as file names rather than the description of the part for the file name. I will detail instructions for an easy method of doing this using Logopress3 in the next post or two.

General tips & tricks for all, LP3 How-To's for users

At some point you may run across a scenario when you try to access a help file within a program, but the help file doesn’t open. Typically you will get a screen similar to the one below saying “Navigation to the web page was canceled” (Windows 7) or “Action canceled” (XP). I believe that this typically happens when you get this help file from somewhere other than a standard installation of a program, and this is Microsoft’s way of protecting you.

What you need to do is navigate in Windows Explorer to the location that the help file is located in, such as below for example.

You then need to right click on the help file and select Properties. Then, on the General tab, select the Unblock button towards the bottom right and then hit apply and then OK.

Now the help file should appear when you try to access it from within your program.

As a side note, some help files can be accessed by double clicking on the help file itself from within Windows Explorer, and others cannot. Some can only be accessed from within the program they written for.

General tips & tricks for all, LP3 Warning messages, Windows tips & tricks

Sometimes you will find that after inserting your BOM, you have the identical Standard Component listed more than once, rather than combined into a single line. Below is an example of a BOM that has 3 different item numbers for what could be a single item number for an identical pilot, as well as 5 different item numbers for an identical nitrogen cylinder that could have a single item number. In the case of the nitrogen cylinder, the 5 different lines total 18 pieces.

The reason for this follows. Some Logopress3 Standard Components are created by Logopress3 with multiple configurations in them, one for each time they are inserted, and others only have a single default configuration in them. Examples of those that have a single default configuration include all screws and dowels. These are inserted with single default configurations because they are standard length items, typically in 1/4″ increments for example.

Examples of those that are created with multiple configurations each time they are inserted into the tool are nitrogen cylinders and cylindrical punches and pilots. Of course these have variable/customizable lengths within them, be that point length or stroke length.

Of course if the pilots are all identical you want them to all be listed on a single line. Likewise for the nitrogen cylinders. But in the case of the nitrogen cylinders, if you have one cylinder that is part number xyz that has a travel of .323 and another with the identical part number xyz that has a travel of .395, then these will need to be listed as two different items in the BOM. If all of the cylinders that are part number xyz have an identical stroke length, then they can all be combined into the same item number. Such is the case for the picture below. I started out by using the search tool in the feature manager tree (see “Filtering the FeatureManager Design Tree” post in the May, 2010 archive in this blog) to search for Kaller. Then, based on what I saw in the tree after this “Kaller” search filter was applied and the quantities I saw in the BOM, I changed the search to “.845″ and so this is what I was looking at.

Since all 5 of the above configurations are identical other than the configuration name itself, I decide to highlight all 5 cylinders in the tree (seed components, not those in patterns, those in patterns will follow the seed automatically) and right click and select component properties as you can see in the picture below.

I then choose to set all the components that are highlighted to the same configuration name – I could choose any one of the ones that are .845 and so I choose the first one that doesn’t have an underscore after the name. Select the configuration name you want them all switched to and select okay.

Side note: (In the picture above you can see that the first two configurations are not 0.845 names but 0.608268. I did a search for 0.608268 in the feature tree and found nothing. This means that the designer at one point inserted this model and this stroke cylinder at this custom stroke length, but then either deleted it or didn’t end up using it. So note that when you open this nitrogen cylinder and look at the configuration property manager there may well be several configurations that are unused.)

After selecting okay, as you can see in the picture below that all instances of the nitrogen cylinder use the same configuration. As stated above, this caused all the patterned cylinders to update to this single configuration automatically.

Now, when you switch back to the BOM you are prompted that the document has changed and you are asked if you want to update the table. Answer yes and the table takes a few moments to update and then looks like this. As you can see, there is now only a single nitrogen cylinder listed and there is a quantity of 18.

LP3 How-To's for users, LP3 Standard Components

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- info for LP3 users

Ditto is a great program for increasing productivity, regardless of what you are using it for. Even simply for filling out forms or whatever, I use it often.

Haven’t you found yourself wanting to copy something to the clipboard by using Ctrl+C and then realizing – “Wait, I also need to copy that, but I can only copy one thing at a time. Nuts!” That’s where Ditto comes in. The picture below is a great example of this. I knew I was going to write this post and I knew I wanted to paste the web address in here as far as where to get Ditto and I also wanted to copy their description of it into here. So I simply used Ctrl+C on both things. Then when I ‘m ready to use one or the other (or any of the last several items I’d copied to the clipboard) I simply press the default key combination to bring up the Ditto box which is Ctrl+~. (That’s the control key plus the key to the left of the number 1 key, and as you may remember from a previous post, this ~ is a tilde.) Here’s a picture of the box that pops up:

Ditto is a free open source program that is very tiny and loads with Windows. I’ve been using it since Windows XP and now use it with Windows 7 Professional and have had no issues at all. You can get it here:
http://ditto-cp.sourceforge.net/index.php

It is extremely simple to install – just use the default options. All you need to remember is to let it start when Windows starts and that way Ditto captures all clipboard entries. Then all you need to remember is that the hotkey to open Ditto so that you can select one of the entries from the list is Ctrl+~. That’s it!

Here’s the official description from the Ditto web site:
Ditto is an extension to the standard windows clipboard. It saves each item placed on the clipboard allowing you access to any of those items at a later time. Ditto allows you to save any type of information that can be put on the clipboard, text, images, html, custom formats, …..

General tips & tricks for all, Software we use, Windows tips & tricks

There’s an awesome and often overlooked feature in SolidWorks that some of you know about and I believe others would really benefit from. It is the filter that SolidWorks added to the topmost part of the FeatureManager tree a couple of releases ago.

As you begin typing, the graphics area updates in real time displaying items that match.

Take note of the options that are available and also note that you can search for anything, including sketches, specific features, etc…

Check it out in the SolidWorks help.

SolidWorks tips & tricks

Hopefully, if you have the occasion to use locking tabs in your die designs you’ve taken advantage of the automated Punch Locking Tab function in Logopress3. If you haven’t, make sure you search the Logopress3 help file for “Punch Locking Tab”.

I’ve just realized today that the help file doesn’t document how to use a Punch Locking Tab with a round punch yet. We’ll get that updated, in the meantime, here’s how:

You need to edit the round punch first and add a flat area to the outer diameter of the punch at the same radial position that you want the locking tab to be at. (You might find that using a 3 Point Center Rectangle in your sketch is efficient for this and then using a CutExtrude…) This flat area will be what you will pick for the “groove face” selection. This flat area can be either at the base of the punch or at the cutting end of the punch and can be as little as 0.001” deep(Sketch dimension) x 0.001” deep(CutExtrude dimension). (Hint – make the depth of the CutExtrude 0.376” deep so you have a nice big target to select for your second pick, which is the groove face. Then, after applying the locking tab, change the 0.376” dimension to 0.001”.)

LP3 How-To's for users