Door/Drawer editor opposite direction?.

[Stephen Tinkler]

Is there still a problem with the door/drawer editor, the exterior profile tool (additional offsets) are ok on screen in ecabs, but put through the supercontrol the tool offsets are in opposite direction?.

This was pointed out with an email in march 2007

Thanks Stephen

[Ryan Hochgesang]

Stephen,

Please provide supporting files to: program@thermwood.com and we will have a look at your situation. We will need the eCab design file (ie: .hsf, .esa or .esj) as well as the EXPORT from Control NESTING and the Actual CNC file you've written.

Thanks!

[Daniel Menard]

I have the same problem... I have to go in the opposite direction to get it to work.

[Ryan Hochgesang]

Stephen,

I have recieved your files and will have a look and get back to you. Thanks!

[Daniel Vonderheide]

I had requested additional files to verify what is happening but have not received them yet so I will try to explain the process and hopefully this will shed some light on the subject.

When you create an mdf door in Ecabinets and send it to Control Nesting, Control Nesting sees profile information in the TWD. When it is time to create the code to cut them, it passes this profile information and the mdf tool information from the settings area to the Profile Modeler. The Profile Modeler looks at the information passed from the settings area and determines if it needs to profile the part or if it is using a custom tool to create a centerline cut. This centerline is important and will be covered in a second. Once PM has this information it will create the path needed to make the part. PM does not look at the cut direction specified in CN and will only create the path as a conventional cut. There is no way to change this direction. Now that PM has created the path, it passes this back to CN and CN applies the code to the program it is creating.

Now comes the important centerline explanation. This information is passed from Ecabinets directly. When you select a tool to apply a profile to a part, you see a representation of this tool in the open dialog box. Now, this dialog box, not the tool, is where ecabinets gets the centerline information. This is where most errors come from. The vertical line that runs in the center of this screen between the blue area and the yellow area is what ecabinets is considering as the centerline. If the tool is designed asymmetrical from this line, and then applied, ecabinets is passing the information that the centerline is at zero with no radius comp or additional offset and the depth is whatever you have set in the plunge depth. This will work for display purposes, but not machining. If a tool is designed symmetrically using the "centerline" in the shape manager, when it is brought into this open screen it will be symmetrical. Then you can apply addition offsets left or right to move it from this centerline. When applied to the part, it now has the correct offset and depth applied to the part which is then passed to the machine in the TWD file.

I hope this has shed some light on the subject.

[Stephen Tinkler]

HI Daniel

This is not a problem to us as we use a door package we just thought we’d point it out because its the second time we’ve came across it, the file attached is of what it looks like in eCABS to what happens after machining,This problem also happens when you use any tool.

Thanks Stephen

[Ryan Hochgesang]

Stephen,

Thanks for all the information that you've submitted as we looked into this issue. This issue has been reproduced and documented.

[Stephen Tinkler]

Hi Daniel/Ryan

When we make a door in the door/drawer editor we don’t save it to a cabinet [we don’t use the custom layout]. We make a door in the door editor save it close it then click load item, click door/drawer enter sizes then click select door, this open in the door drawer editor select the door click OK,this opens the door to the cabinet assembly editor, then press CNC to create the file for the machine. This is the procedure we have been using.


Thanks Stephen

[Daniel Vonderheide]

Currently, the way to get the results you want are to create the tool with the correct diameter for the offset you want and then use the apply radius comp instead of the additional comp. This will display the part correctly in ecabinets and will also create the cnc code as a centerline on the edge of the door with tool comp codes turned on. You will only need to make sure that the tool diameter in tool management is set for twice the offsert you want and not the actual tool diameter. In the pics above, you have the tool comped at 2.3mm even though it is a larger tool. You wound need to draw this tool and then define the diameter as 4.6mm. In tool management you would set the diameter of the tool to 4.6mm so it would comp out the 2.3mm. Hope this helps.

[Stephen Tinkler]

Hi Daniel thanks for the reply
On trying this out we have found that the apply radius comp does not work in the tool dialog box in the door/drawer editor,but it only works in the part editor.

Thanks Stephen

[Daniel Vonderheide]

I apologize, I left out a small but important bit of imformation. Your tool will need to be drawn with the offset already applied to the tool so it displays correctly. This means that if you are wanting a 2.3mm offset to the left, then the tool needs to be drawn with the center of the tool 2.3mm left of the zero line. This will have it display correctly in ecabinets and then the radius comp button will cause the machine to turn on compensation for the tool diameter with no additional offsets applied.