What can I do with this software?

If you have list of rectangular parts (cut list) that need to be cut from sheet of material and you want to minimize your waste, this software can help you. This is not a professional software. There are other programs that can do the job, probably more efficient. However this one is free. At the time I created it there was not a free version that could do what this program does. It can draw DXF files with the optimization patterns, OR/AND write G-code programs to run the cut on a CNC router.

What do you need to prepare?

You need to create a cut list and save it as a CSV file. Please, download the sample CSV input file (cutlist.csv) and edit it to create your own list. You can change the file name and the contents of the file, but keep the header line and don't delete or rearrange columns.

Which fields need to be filled in the form?

Regardless of what you need, DXF files or CNC programs, or both you need to enter the sheet size. ("Sheet Length" and "Sheet Width").

Do I need to enter "Sheet Thickness"?

Yes you need "Sheet Thickness" if you select CNC programs output. You don't have to enter the actual material thickness if you are not planning to cut the parts through. You might want to leave "Onion Skin" (some uncut material to hold the parts from moving and finish the cut with a hand trim router).

What is "Border Trim"?

Assuming your sheets of material have rough edges and the optimization should move away from these edges by certain length. You can enter "Border Trim", that is the offset from the edges of the sheet that will not be used for the parts to be cut. It needs to be a positive number or zero. It can have decimal fractions. Keep in mind - the optimization might not work if the trim is taking too much from the sheet and there is no enough material left to cut your parts.

What is Kerf"?

"Kerf" is a term used when cutting with table saw or panel saw. Here it means the minimum distance between the parts in the optimization. It can be zero if you are planning to cut with a laser. If you are using a router bit I recommend enter at least the diameter of the bit. The number entered in the field "Lead In Start Offset" if it is more than zero should affect the "Kerf" too.

What is "Grain"?

Some materials like wood have patterns that have direction. If you need to maintain that direction in your parts (Part Length to be parallel with Sheet Length and Part Width to be parallel with Sheet Width) then you need to select "Grain".

Do I need to label my parts?

"Label Parts" is an option available for the DXF file output. It will create a text field and write the "Part ID" in that field. The part ID is the text you put in the CSV input in the "ID" column. That could be identifier for the part so it is easy for you to sort them out after cutting.

Do I have to enter Label Font Size?

Yes if you have selected "Label Parts" you have to specify the size of the font. That will be the height of the characters in the text field. I suggest you choose font size that will be easy to read, but not too big to obscure the parts.

In what units is the "Feed Speed"?

It depends on your CNC machine setup. If it is imperial units setup then the feed speed is inches per minute, in metric setup will be meters per minute. If you are not sure what speed to use, refer to the router bit specs if available or do search on feed speed and chipload.

What is "Lowering Speed"?

It is the Feed Speed while the router moves in Z axis. When entering the material to start routing and when exiting the material after finishing the current route. It can be set to a lower value then the "Feed Speed" in order to avoid damaging the material on impact or if the Z axis have lower speed capabilities.

What is "Z Clearance"?

It is how much space you need to safely travel above the material you are cutting. The router will raise that high above the top surface of the material and fast travel to the next route.

What is "Lead In/Out Angle"?

This is the angle of the trajectory of the tool while lowering to enter the material to the XY plane. Same angle apply to the trajectory of the tool emerging from the material.

What is "Lead In Start Offset"?

If you are using a compression route bit you might consider to offset the entrance point of the route from the part edge in order to avoid chipping it from the up-cut part of the compression tool. This offset applies to the start position at Z clearance height. It means the actual entry point of the tool will be offset less. For example if you are routing 0.75" deep and your Z clearance is 1" and you have entered 0.25" for "Lead In Start Offset", the actual entry point will be offset from the part edge by approximately 0.107" ( 0.25 * 0.75 / 1.75 ).

What is "Number of Passes"?

You might want to do your cutting gradually in multiple passes. Based on the CNC router speed or capabilities to remove material or the router bit chipoad or if the material fastening to the bed you should decide how many passes to do to cut your parts. The "Material Thickness" will be divided on "Number of Passes" and each pass will increase the route depth by the result of the division.

What is "Last Pass Thickness"?

I find this option useful when there is a risk of your parts moving at the end of the route. It gives you control of how much Z increment to make in the last route pass. That will automatically recalculate the rest of the passes increments. Aim for a value that is small enough to lower the chance of moving, but is big enough so it will not release the part before it is cut.

What is "Tabs"?

These are small portions of the route left uncut, so your part don't move before the end of the program. Be careful the tabs might not serve their purpose if the parts are close to each other. The tabs on the first part might get cut by the route of its neighbor's parts. In order this to work you will have to increase the "Kerf" and the "Border Trim".

What is "Tabs Width"?

It is exactly what it says. It is the distance from the point where the router rises a bit to the point where lower back down to the final routing depth in order to leave a "Tab". You cave to take into account the geometry of the router bit impact to the "Tab". The actual uncut portion will be "Tab" value minus the router bit diameter. The rise and lowering the router will be done with the same angle as "Lead In/Out Angle" with "Lowering Speed".

What is "Tab Thickness"?

I think this is self explanatory, but it is worth mentioning the tabs are formed at the last pass. If you have set to multiple passes and enter a value for the "Last Pass Thickness", please make sure "Last Pass Thickness" is bigger or equal to "Tab Thickness". Other wise you will end up with "Tab Thickness" equal to "Last Pass Thickness". Good practice is to avoid using "Last Pass Thickness" if you have "Tabs" checked.

What is "Tabs to Cut Ratio"?

There has to be a way for you to control how many tabs to leave on each part. However each part comes with different size, and one set number might not work for all parts. By setting "Tabs to Cut Ratio" the optimizer will calculate how many tabs to make based on the part perimeter length the "Tab Width" and the "Tabs to Cut Ratio".

Where should I set my Z axis zero coordinate?

The programs assume your material top surface as Z=0. The positive direction of Z axis is away from the material (Upward).

Do I need to enter "Router Bit Diameter"?

You do, if you are routing. The CNC programs created here are not using tool correction. Instead the route geometry is calculated to offset from the part edge with the amount of the Router Bit Radius = "Router Bit Diameter" / 2.