Sheet Layout - a couple things

[mattyfatbags]

Sheet Layout - a couple things

I'm working on getting Sheet Layout to help me build cabinets. A couple issues I've run into so far:

1. How does Sheet Layout handle WIDTH X LENGTH? For example, I have a part that is roughly square. Sometimes width > length and sometimes width < length. Does this matter? I was assuming width would typically be less than length.

2. I noticed the Alibre version of Sheet Layout is limited. Specifically, there is no CNC support. Has anyone upgraded to the Commercial version to get G-CODE programming? Will they modify or create a post-processor if needed? What is support like, etc?

 

[WoodWorks]

You need to establish your own convention in Alibre as to which direction is Width and which is Length. We create our parts with the Length along the X axis, and Width along the Y Axis. Of course Length is always along the direction of the grain, and generally horizontal with most sheet optimizing software (more recent versions allow rotating the sheet with the long direction vertical, but the horizontal direction is easier to visualize).

We always create our parts as if they have grain, but the Width & Length issue is less relevant with non-grain sheet goods such as MDF or melamine faced material. One reason for always assuming grain, is that occasional the material changes during the course of design, and we hate to be caught unprepared when a grained material is substituted for one without.

One item that often comes up is that Sheet Layout nests all parts as if they were rectangular and based on the width and length dimensions. Shaped nesting requires a much higher priced program.

I do not know if the CNC Commercial version has been released and would like to know if it is available. How about ShopBot code, or do you have a machine that uses G-Code? DXF output from Alibre can be easily sent to vendors that provide CNC cutting services and they usually will not run code generated by others (too much risk to their machine).

Sheet Layout is great for creating cutlists for manual cutting, and a lot faster than laying out the material by hand.

 

[mattyfatbags]

You have a CNC, right? What program(s) do you use to take a cabinet project in Alibre through optimization and G-CODE programming? Sounds to me like it isn't Sheet Layout.

 

[WoodWorks]

We do not actually own a CNC machine ourselves (the wife said no again today as I was browsing the used ShopBot listings), but we create DXF files to send out to CNC machines, and we use MasterCAM to generate CNC code for a regular customer that owns two shopbots.

My wife used to write G-code for her ex-employers KOMO CNC and the shops metal working CNC that was used to build custom machines. But there are many flavors of G-Code, based on the vendors enhancements.

We use Sheet Layout and CutList Plus (based on customers preference) for those jobs that will be manufactured without CNC, and MasterCAM for those jobs that will be manufactured on a ShopBot. We send out the DXF files for use by job shops that have their own nesting software, and the Thermwood CNC machines will nest all DXF files automatically with the built in controller software. They have a very nice layering scheme that is easy to support with Alibre.

We are providing DXF files and ShopBot code for cabinets that use BlindDado joinery, and where the CNC mills all holes and pockets. These models are bit slow even on an AMD Athlon X2 6000+, but when it comes off the CNC it is ready to assemble with puzzle like precision and does not require any secondary operations such as biscuits for pocket screw holes.

On the other end of the spectrum, we use a much simpler and faster model for creating rectangular parts that will be cut on a table or panel saw and assembled with screws or other fasteners. Here we do use Sheet Layout as it provides faster nesting results than by hand. We also use sheet layout to do preliminary nesting of CNC jobs to get an estimate of material quantities required.

A good program for creating G-Code (or ShopBot code) is VCarve Pro. It is quite powerful and affordable, but does not yet have nesting capability. Unfortunately, to get nesting and code generation, you are probably talking at least $3500. We looked at ArtCAM, EnRoute, AlphaCAM and finally bought MasterCAM. The cost was justified by the ongoing use with the ShopBot customer. Once VCarve Pro adds nesting, or Sheet Layout releases the Commercial Version with code generation, the big guys will have to watch out.

While I keep drooling over the used ShopBots, I will probably not be purchasing a machine myself as there is such a large community of ShopBot owners available to do contract work, various other job shops willing to do CNC work, and quite a few Thermwood job shops available for work through the eCabinets network. Besides, we started doing design work for other shops because I got tired of lifting sheets of plywood in my own shop. Ideally, I would get a lift cart, and better yet let the eldest grandson shove the material around the shop. For now I will continue to labor over Extrude Boss and Cut, with many Linear Patterns to create joinery and multiples of parts for custom Kitchens and Entertainment Centers.

 

[WoodWorks]

The DXF file export would probably be the best feature to begin with, as the fully nested material outlines could be saved to DXF, and then imported into VCarve Pro (or other code generating software).

You could probably use Sheet Layout and print the layouts to a PDF file, use a PDF to DXF conversion program, and then open the DXF files and create the code with VCarve Pro. The people that wrote VCarvePro used to work for a large CNC software provider, and saw the trend to more affordable software, started their own company and are providing CNC coding software with multiple machine drivers along the lines of Alibre's lower cost software business model.

So, create the nesting with Sheet Layout, and code it with VCarvePro until Sheet Layout provides an all in one solution.

We use MasterCAM with our own custom scripts to nest cabinet parts quite efficiently and create ShopBot code. We also output DXF files for custom projects that require milling more complicated than our "nested based manufacturing" solution. We then let the CNC operator use their copy of VCarvePro for the one off specialty milling, engraving, and work that does not fall in our narrow scope of nesting cabinet parts.

We are glad to share the details of how we get our work to CNC code. Start with our techniques and standards posted at the Instructables website, and we can then discuss the nitty gritty of getting the model into a "CNC" drawing, layer the lines into toolpath's, and finally getting the DXF out to the file system without loosing data every time the model updates the drawing.

 

[skeller]

Is there anyway to automatically export all the DXFs from a complete assembly; for example a kitchen? It would be nice to be able to export all the sheet stock dxfs at one time and avoid having to go to every single part in every cabinet assembly to get it done. That would be a sure way to miss something.

Any suggestions?

Thank,
Steve

 

[WoodWorks]

We output the BOM and use that as a guide for the parts that need DXF files to be created. Unfortunately, the DXF files are created from a Drawing of EACH part and these drawings should be checked for problems before output.

While I often write scripts, and hope to automate this as much as possible in the future, the current DXF output via the drawing needs visual verification before output.

Also, this is the case where you already have a CNC drawing from which to create DXF files for each part. If you have special shaped parts, and not something of a standard cabinet, you will have to create the CNC Drawing for that part in order to output the DXF file.

With CNC manufacture, you also need to consider what parts will be manufactured face up and face down, based on the joinery and holes. Some parts like Top and Bottom, will need to be milled both sides when there are vertical dividers in a Cabinet.

I have seen some conversion software that will output a DXF file from an Alibre Part file, but have not tried this. Since there is no way to specify a layer in a part file, I have not pursued this method because we use layered DXF files, where the layer determines the depth of cut. It would be nice to get a layered DXF file directly from the Part file.

 

[mattyfatbags]

I just found out Sheet Layout does not offer a CNC version. I was hoping to upgrade from the Alibre version of Sheet Layout to the CNC version so that I could input a BOM from Alibre into Sheet Layout and have it spit out G-CODE. But just like everything else with Alibre, there's much more arm twisting involved to get the desired result.

Bottom line is that I'm looking for one of two alternatives. First, I'd like a program that can take as input a CSV formatted BOM that I export from an Alibre design, and have this software optimize and generate GCODE. The second alternative is a program that simply does optimization and can output DXF files of the optimization. I can then take these DXF files into BOBCAD and generate my GCODE there. I was hoping Sheet Layout was my solution, but it's not. Anyone know of an alternative that is relatively inexpensive. Since this is just rectangular shape optimization (not true shape), I would expect it's got to be a fairly simple algorithm so it should be a cheap program.

If I can't find one for a decent price, I would think it wouldn't take too much time to write an Autocad VBA app to take a CSV formatted BOM and write an algorithm that sorts through and creates the geometry you need to then take into BOBCAD to produce G-CODE. But maybe I'm wrong.

 

[WoodWorks]

I have done some preliminary research on creating 3D DXF files from the Alibre STEP file output. My initial obstacle was defining the layer for the geometry, so I created a convention where I provide the layer name as part of the Sketch or Feature name by including it in special brackets. I use the [] to contain the layer name for a feature and the {} braces for a layer name for a sketch. That way I can create a program to create a layered DXF from either Sketches or Features.

However, we are so busy cranking out the work using DXF output via drawings, that I have no time to spend on developing the script and program for this.

I have seen a conversion program to create a DXF file from a Part File, but it since there is not any layer information in Alibre, it seemed that it would be a step backward from out current layered DXF output. We want to avoid having to toolpath each project in the CNC software.

Currently, once we create the original CNC drawing and toolpath it, the tool path information adjusts with changes to the part size and we do not have to tool path any of the features again. Since we create new cabinets from our standard template (that contains these layered DXF drawings), the new cabinets include the pre-defined DXF output drawings. Once we complete the cabinet, we open our CNC Drawings, let them update, fix any toolpaths that lost constraint, and Export the layered DXF for nesting and coding. A bit more work than I would like, but still a lot faster than doing hand coding or tool pathing each part in the CNC software.

With our cabinet template models, we can create cabinet designs nearly as fast as dedicated cabinet software. But we have the flexibility to create joinery and designs not yet programmed into the capabilities of most cabinet software. We moved to Alibre because our cabinet software did not provide graphics for every feature of the cabinet, and sometimes we had to take some details of our design setup on faith. Usually that faith was misplaced and we longed for true graphical verification of our designs. Alibre has provide that graphical verification. While this works for our one of a kind custom work, it is probably not as fast as using cabinet software to do everyday vanilla cabinet production. Then again, the cost of cabinet software able to do more than cabinets is quite expensive.

 

[mattyfatbags]

Kirk,
Maybe we should take a step back because I don't really follow what your work flow is. You said that you sub out your CNC work. So what do you send to the CNC guy? Do you send a DXF file with OPTIMIZED layouts? Or do you just send DXF files with the individual parts and have the CNC guy do the optimization?

I could be confusing terms, but by "optimization", I mean optimizing the layout of many parts on a single 48 x 96 sheet. I think nesting means the same thing but I could have my terms confused.

We have a CNC but we currently only use it for curved parts. We mill all our cabinet parts on the table saws. Anyway, our work flow with parts that we do CNC is to manually lay them out and then manually generate the tool path G-CODE in BOBCAD. This process is way too slow for cabinets. Actually, generating the G-CODE from an optimized layout is pretty quick. The bottleneck is in doing the optimization (or nesting or whatever the term may be).

The expensive cabinet programs (SOLID, etc) do their optimization from a CSV file that the design portion of their software generates. And since Alibre can generate a CSV file via the BOM export, all I should need is an optimization program to generate an optimized layout in DXF format that I can then take into BOBCAD for programming.

I think I'm repeating myself now. Just want to be as clear as possible. Anyway, bottom line is that I'm interested in knowing how your optimized layout is generated. Thanks.

 

[WoodWorks]

We are currently doing Design only work for others. Our small family shop is sitting idle, except for personal projects and honey-do mandates. We have had such success with our Alibre Design work, that my wife and I derive our entire income from custom cabinet design services using Alibre Design.

We now use our own woodworking experience to provide contract design software services to others. Rather than just being drafters, we offer design services as experienced woodworkers. And since we spend all day long using the software, we are able to maintain a high level of expertise and efficiency. One of our customers often needs a bit of a refresher course after spending 6-8 weeks actually building the projects we worked designing together. It is hard to maintain proficiency when away from any software for an extended period of time.

We do custom design work using standard models we created. Combining the CASE with the FACE (and drawers if necessary), we create a CABINET assembly. The cabinets are sub-assemblied into an ELEVATION, which is combined with a SITE model to create our top level INSTALLATION model. From the INSTALLATION, we create Shop Drawings for client approval. A standard part of the individual Cabinet models are a detailed dimensioned Drawing with sections and details of that specific cabinets. Also, the CNC drawings which we use to output the DXF files are a standard part of the template. We have pre-configured layered DXF files that have the geometry of the main features on specific layers. Once the model is updated, we only have to open the CNC drawing, let it update, verify that it is still valid, and export the DXF. While it is a tedious job, it goes rather quickly to run down through the CNC drawings in order and Export the DXF file. A bit of upbeat music without lyrics helps keep brain death from setting in during the output of an entire Kitchen. It helps greatly to be organized and repeat the same process over and over again without errors. I will often change out the work and output a single elevation (or two) and the do a bit of new design work before going back to finish another elevation.

Once the DXF files are created, we combine those files with a BOM from Alibre and import them into MasterCAM to do the nesting/optimization of a single cabinet or entire job of cabinets. The selected CNC code output is automatically created during the nesting. We do have some control in MasterCAM as to the arrangement of the nesting, but sometimes it would be nice if I could shift a part slightly manually. However, the rapidity of which an entire job can be nested and code output is worth a little material waste over the perfect manual nesting.

There currently does not exist the affordable alternative to nesting/optimization comparable to the value provided for design by Alibre Design. However, I have created a manual "nesting" assembly with a "96x48 sheet" part, onto which I drop cabinet parts and re-arrange them into a nesting pattern like using cutouts on graph paper. Once completed, I suppressed the base sheet part, and output the resulting nesting to a DXF file. You could also use Sheet Layout to provide a guide to the part nesting so that you would not have to determine the best nesting by trial and error.

 

[mattyfatbags]

Now that's the detail I was looking for. Thanks, Kirk.