nestfab nests coded wrong

[jmajorg]

Hello,
I am new to Sheetcam and have written a post for our laser cutter. I have a seat of Nestfab for nesting parts and it outputs a large dxf of the nest it generates. I made a Nestfab nest that consisted of 24 six armed flex disks. There is a hole in the middle of each part and another on each of the six arms of each part. I can import the nest dxf into sheetcam but when I post code from the nest it cuts the profile of each part before cutting the part's holes. It is consistent in that each part is finished before starting another. My post is outputting code with the correct syntax for the laser. Is there a setting I am missing. Sheetcam is a wonderful program and I am going to continue using it on jobs are nested normally. It would be great though if there was something that could remedy the profile first problem.

Thanks

[Les Newell]

There are a few possibilities here. First of all, is the hole on the same layer as the outside? If so, edit your cut operation and go to the 'Cut path' tab. Make sure you have optimisation set to 'Auto' and and set the cutting rules to 'All inside first' or 'Keep parts together'. For your application I'd recommend 'keep parts together'.

If the hole is on a separate layer you probably have the operation to cut the outside before the operation to cut the inside.

[jmajorg]

Les,

That fixed the problem. The optimization was set to "manual" so I set it to "Auto" and the cutting rule was already set to "Keep parts together".

Could I have manually optimized this large multipart nest so that I could define the order that the parts were cut? Most of the time the auto optimization will work, but there will be times that I would like to determine the part order. What would work well is have a basic operation for inside cuts and one for outside cuts. Probably

[jmajorg]

Les,

That fixed the problem. The optimization was set to "manual" so I set it to "Auto" and the cutting rule was already set to "Keep parts together".

Could I have manually optimized this large multipart nest so that I could define the order that the parts were cut? Most of the time the auto optimization will work, but there will be times that I would like to determine the part order.

Sometimes we like to tab the outside of the part to keep it from tilting. We have found that one tab on the profile of a part will keep it from tilting excessively. Any more make removing it from the skeleton more difficult and cleanup is longer. I tried a negative overcut and that did leave a tab, but it also tabbed all the small holes inside the profile which is not desirable. I looked at the "Holding Tab" dialog which would give us the ability to limit tabs to the outside profile only, but a problem that I can see is holding tabs are put in by some algorithm and can be anywhere. This would likely require two pierces, one of which would not have a leadin which is not desirable. What would work well is have a basic operation for inside cuts and one for outside cuts.

Again, I think you have created a very capable and inexpensive CAM solution. Used along with Nestfab it make a package that fits our needs better than many of the expensive mainstream solutions. I expect to buy two more seats to use at our machines and allow the operator to program his machine.

Thanks for your help.

[Les Newell]

Could I have manually optimized this large multipart nest so that I could define the order that the parts were cut? Most of the time the auto optimization will work, but there will be times that I would like to determine the part order.

Yes you can. Take a look here https://www.youtube.com/watch?v=2bi_wU-jPYk

Sometimes we like to tab the outside of the part to keep it from tilting. We have found that one tab on the profile of a part will keep it from tilting excessively. Any more make removing it from the skeleton more difficult and cleanup is longer. I tried a negative overcut and that did leave a tab, but it also tabbed all the small holes inside the profile which is not desirable. I looked at the "Holding Tab" dialog which would give us the ability to limit tabs to the outside profile only, but a problem that I can see is holding tabs are put in by some algorithm and can be anywhere. This would likely require two pierces, one of which would not have a leadin which is not desirable.

One option would be to put the outside cuts on a different layer. You can the use the negative overcut option. Alternatively you can manually place tabs. Select Mode->Edit tabs. Make sure the operation you are interested in is selected then click on the outline wherever you want a tab. If the tab is over a start point you will get only one pierce.