Applying Template using old CNC Bit info

[TSmith88]

I'm using the "Apply Template to All Sheets" gadget, and I've been adding a Square off cut and trying to save the files, it gives me this error:

Toolpath Error

What is causing this error? It looks like the template is not applying the information that is currently set in my tool database.

Tool Info in Database

Tool Info Adding from Template

[adze_cnc]

It might be better to see a screenshot of each toolpath mentioned in the error to verify that the same bit is selected for each toolpath. Sounds like you have tool x for one and tool y for the other.

[Adrian]

The tool information is copied over to the toolpath when it's created. There is no link from the toolpath to the tool database at that stage. If you create a toolpath and save it as a template on Monday (for example) and then change the tool definition in the tool database on Wednesday and create a new toolpath with that tool when you load the template the software will treat them as two separate tools.

You have two different diameters so it looks like you did something along those lines.

[TSmith88]

If I'm understanding Adrian correctly, the tool information is static to what was in the system when I originally created the template, so it does not update when I change the bit diameter? Is there a way to set up a template that will toolpath imported AutoCAD vectors based on their layers using CURRENT tool information in the database?

It's my thinking that you create the template and assign the tool, if you're assigning tool#1 there should be a way to have it take tool 1 from the CURRENT tool database, instead of the outdated tool database that was in use when originally creating the template? Or is there a way to update the tool information within the template to the current tool information before I apply the template? The point of me creating the toolpath template was to be able to just hit "Apply Template to All Sheets" and save time not having to toolpath every vector, of every sheet, every time. I'm sure there's something simple I'm not seeing, if anyone has some advice on how I could accomplish setting a template that will stay current, or at least have the ability to manually update that template to the current tool information for when I swap bits out?

[Adrian]

Your

The point of me creating the toolpath template was to be able to just hit "Apply Template to All Sheets" and save time not having to toolpath every vector, of every sheet, every time. I'm sure there's something simple I'm not seeing, if anyone has some advice on how I could accomplish setting a template that will stay current, or at least have the ability to manually update that template to the current tool information for when I swap bits out?

That is the correct use of the template. You don't need to toolpath every vector of every sheet. You associated the layers in the toolpaths, save them as template and load them then use recalculate all to create the updated toolpaths.

What you seem to be wanting to do is to create one template and then use it for different types of tools. That's not how it works. You need a toolpath for each different type of tool and you can have many toolpaths in a template.

You don't update the template when you swap bits. The use of the different sized bits is part of the toolpaths within the template. If you have an existing template setup for (as an example) a 1/16" bit, a 1/4" bit and 1" v-bit and you want to change the nearest metric sizes you would need to create a new template.

[TSmith88]

That is the correct use of the template. You don't need to toolpath every vector of every sheet. You associated the layers in the toolpaths, save them as template and load them then use recalculate all to create the updated toolpaths.

What you seem to be wanting to do is to create one template and then use it for different types of tools. That's not how it works. You need a toolpath for each different type of tool and you can have many toolpaths in a template.

You don't update the template when you swap bits. The use of the different sized bits is part of the toolpaths within the template. If you have an existing template setup for (as an example) a 1/16" bit, a 1/4" bit and 1" v-bit and you want to change the nearest metric sizes you would need to create a new template.

I do not want to create one template and use it for different tools. What I want is to create a template that pulls my Tool values from the current database, keeping all the diameters of my tools consistent with what is currently in the CNC when I use the template. If I import my vectors, create nest, and apply template to all sheets I want it to use my template and pull in the current tool information of what is actually in the CNC.

Maybe I'm not understanding something. Here's the process I went through:

1) Import AutoCAD file.
2) Select desired Vectors.
3) Create Nest
4) Apply Template to All Sheets
5) Go to sheet with excess space, Add Remnant Cut Line.
6) Toolpath Remnant line using Tool 1, Profile cut ON line.
7) Attempt to save.
Get Error as described above.

Here is an example of one of the sheets I was trying to GCode. The blue line is on layer "Cut Out (Panel Goods)" the magenta lines are on layer "1/2 Pocket." I then manually added the remnant cut using the line command in VCarve and added a profile toolpath using tool 1. Then when I tried to save the new toolpaths for the sheet I got the error.

Here are the toolpaths I have set up in the template, the name of the toolpath matches the layers associated with the toolpaths. Both of the highlighted toolpaths are using tool #1, the only difference is one is on the inside of the vector and the other is on the outside.

Maybe I didn't create the template properly if it's not pulling in the current bits, so how can I update this template so every time I use it, the tool information is accurate to what is in the tool database?

[Adrian]

You can't create a template that changes the tool information in the template to be whatever it is now in the database. As I said earlier when you create the toolpath the tool information then becomes part of the toolpath. When you save a template it consists of one or more toolpaths so there is no link to the database.

What I don't understand is why you are changing the diameters of the same tool definition. If you have a 3/8" tool that is 0.311" (for some reason) and another that is 0.362" then they are different tools so need different tool numbers. If the template and the new toolpath have different tool numbers then you won't get the message but your post processor must be able to handle tool changes.

If you want to update the template to use the new definition then you have to edit the toolpath, select the new tool from the database and recalculate the toolpaths before saving the template with the new definition.

[TSmith88]

The reason I'm changing the diameters of the tools is when they are replaced with new bits or sharpened bits the tools have a new diameter from the tool that was in the database.

If I'm understanding you correctly, I will have to create a new template every time I change the bits out, or every time I import a job. There is no way to have a template that pulls information for the tool from the database. When I create a template all of the tooling is static with no way to update outside of recreating the template before I apply it to all sheets, or creating a template for each job I nest as opposed to a "master template" which is what I've been trying to do.

Maybe I'm overlooking a better way to achieve my goals of setting up a master template to use for all of my imported AutoCAD files. I only noticed this the other day when I was adding the remnant cuts, but I guess the countertops I've been sending out have all ended up using the outdated bit information, but didn't cause any problems so no-one told me about it.

[Adrian]

The reason I'm changing the diameters of the tools is when they are replaced with new bits or sharpened bits the tools have a new diameter from the tool that was in the database.

That is usually handled by cutter compensation in your control software not the CAD/CAM software. You set the difference between the tool size you've programmed and the actual tool in the control software and it adjusts the paths to suit.

If your control software is not capable of it you might be able to do a similar process by using the offset in the toolpath and document variables to control it but it's not something I've tried.

[TSmith88]

That is usually handled by cutter compensation in your control software not the CAD/CAM software. You set the difference between the tool size you've programmed and the actual tool in the control software and it adjusts the paths to suit.

If your control software is not capable of it you might be able to do a similar process by using the offset in the toolpath and document variables to control it but it's not something I've tried.

When you say control software are you referring to the control on the CNC machine? I am not familiar with this CNC at all, I'll have to ask the CNC operator if it's capable of that. At my old shop I was responsible for programming it and operating it, at this shop I have no experience operating it. I just program the files and hand the cut sheets to the operator.

If I have to use the offset and then recalculate all of the toolpaths it would be the same problem of the template not working for what I need. What I want is to create a template, and use that template for all future jobs. What I would really like, and would be a MASSIVE help for me would be if the template would pull the information from the current database. There could be a verification for "Which tool group was used for this template?" Select the tool group you need and then when you apply the template it looks at the toolpaths and looks at your tool database for the current information. "Toolpath in template calls out tool1 for this, User selected tool group X, pull tool geometry information from current tool database." Obviously I'm not a developer so I don't have a clue of how complicated this would be to add, but I certainly would love it if the program worked this way.

It seems like what I will have to do is import my vectors from AutoCAD, and create my template for that job. Or maybe I can load my template and update the values then save over my existing template and then apply template to all sheets. I don't see how creating a template and using "Apply Template to All Sheets" helps, if it's not pulling current tool geometry though and you have to create new templates when you change bits.

[Adrian]

When you say control software are you referring to the control on the CNC machine? I am not familiar with this CNC at all, I'll have to ask the CNC operator if it's capable of that. At my old shop I was responsible for programming it and operating it, at this shop I have no experience operating it. I just program the files and hand the cut sheets to the operator.

If I have to use the offset and then recalculate all of the toolpaths it would be the same problem of the template not working for what I need. What I want is to create a template, and use that template for all future jobs. What I would really like, and would be a MASSIVE help for me would be if the template would pull the information from the current database. There could be a verification for "Which tool group was used for this template?" Select the tool group you need and then when you apply the template it looks at the toolpaths and looks at your tool database for the current information. "Toolpath in template calls out tool1 for this, User selected tool group X, pull tool geometry information from current tool database." Obviously I'm not a developer so I don't have a clue of how complicated this would be to add, but I certainly would love it if the program worked this way.

It seems like what I will have to do is import my vectors from AutoCAD, and create my template for that job. Or maybe I can load my template and update the values then save over my existing template and then apply template to all sheets. I don't see how creating a template and using "Apply Template to All Sheets" helps, if it's not pulling current tool geometry though and you have to create new templates when you change bits.

Most control software can do cutter compensation and it's by far the best way to handle it.

If you could set something up in VCarve using document variables as I suggested then all you would need to do is change the document variable and then press the recalcuate all button. You wouldn't need to individually select and change the toolpaths as you're doing at the moment. I've tested it and it does work. You're prompted to recalculate when you change the document variable.

[TSmith88]

Most control software can do cutter compensation and it's by far the best way to handle it.

If you could set something up in VCarve using document variables as I suggested then all you would need to do is change the document variable and then press the recalcuate all button. You wouldn't need to individually select and change the toolpaths as you're doing at the moment. I've tested it and it does work. You're prompted to recalculate when you change the document variable.

How can I set up a template using document variables? And how can I use them for the tool diameters? I've never done any document variables.
If I'm doing a nested job with multiple sheets, would I then have to save all the toolpaths per individual sheet, or is there a way to resave them all at once?

I'll have to contact tech support and try and figure out how I could do cutter compensation as you suggested, I can see that being the best option if it's something I could do at the machine level. Just to verify, if I were to use that method I'm assuming it would be best to set my bits in VCarve statically as easier to remember values such as 3/8" bit being .375" permanently.

[Adrian]

If you use cutter compensation then you set the tool database as the correct diameters so you always know where you're working from with compensation/offsets.

To use the document variable method you go into the Document Variables form on the Edit menu and create a new variable called whatever is appropriate, CutterComp for example. You then go to each toolpath and enter {CutterComp} into the Allowance offset field.

Once you've done that for all the toolpaths then you save the template in the usual way using the Save All Visible Toolpaths as Template icon.

Now when you want to use the template you load it in the normal way and after all the toolpaths for each sheet have been automatically created you then go back to the Document Variable form on the Edit menu and change the value to allow for the difference between the real cutter width and the value in the database. Once you've done this you will get a message saying which toolpaths are affected. You then click the Recalculate all button and all the toolpaths are recalculated with the new offset value.

[TSmith88]

If you use cutter compensation then you set the tool database as the correct diameters so you always know where you're working from with compensation/offsets.

To use the document variable method you go into the Document Variables form on the Edit menu and create a new variable called whatever is appropriate, CutterComp for example. You then go to each toolpath and enter {CutterComp} into the Allowance offset field.

Once you've done that for all the toolpaths then you save the template in the usual way using the Save All Visible Toolpaths as Template icon.

Now when you want to use the template you load it in the normal way and after all the toolpaths for each sheet have been automatically created you then go back to the Document Variable form on the Edit menu and change the value to allow for the difference between the real cutter width and the value in the database. Once you've done this you will get a message saying which toolpaths are affected. You then click the Recalculate all button and all the toolpaths are recalculated with the new offset value.

Just so I understand this. I'll set my 3/8" bit as .375" then down the road if my CNC operator changes the bit out, and now it's .342" I change the document variable to (-.033"). And it for some reason it's larger I would have a positive variable.

Sorry, I know I'm being a bit of a pain with all the questions, I'm just trying to gain a better understanding of the program so I can be certain when I send GCodes to the CNC, I know for sure my parts will be accurate. If I'm understanding this correctly I believe I would need this Document variable for each tool in my template then. If that is the case, then I can work with this method easily. Not a perfect solution, but way better than having to create a new template for each job.

Thank you so much for your help, it is greatly appreciated and will save me a HUGE amount of time in the future.

[Adrian]

That's correct and yes you would need a different variable for each different tool in your toolpaths so if you were using a 1/8" tool, a 1/2" tool and a 3/8" tool you would need three different variables but you've only got to set them up once.