Engraving

[johnnyg]

I have been trying to figure out how to engrave these drawings that i downloaded from here with no success. See attached files. I have tried all these programs and cannot seem to create a tool path to engrave lettering. SOLIDWORKS 2015 x64 Edition, ArtCAMPro, Autodesk Inventor Professional 2016. I can create a tool path to cut holes and the outline of the drawing but no lettering. Can anyone steer me on the right path? Maybe a good diagram of what you have done would be helpful to try to follow it. Thank you very much for any help you can assist me with.

[Jan737]

Hi
We need a bit more information.

Do you want the lettering CNC engraved or with a lasercutter?
If CNC: What software program are you using whit your CNC machine?
Load your drawing as dxf file and your CNC software calculate the tool paths.
Normally this software is able to do the job just by selecting the engrave option. The program calculate the tool path and there you go.


Regards

Jan

[blueskydriver]

Does your setup use or can it use MACH3 for the actual CNC?

John

[johnnyg]

Yes I am using Mach3 for software and yes I will be using a routed cnc mill not laser.

[jonesthesoftware]

Hi johnnyg
If you have Artcam this can make your cnc file.
Because you have Autocad drawings the text is in Simplex which is no good for engraving.

From Artcam use the open file command and select the .dwg file and open the drawing (you can open a pdf file but you will need to resize it to the actual full size of the panel to make the cnc toolpath as obviously you will be working on a full size panell)
Now use the TEXT tool on the assistant page to put the text on the page in the correct position.
Boeing font is Futura lt Bt ( you need to have this font in your winsdows font folder already.
You can download it from the internet.)
When you select the text tool you will see options for size(use about3-3.5mm) as well as character spacing, line spacing etc.
Experiment with these to get the desired effect.
You can move the text and use the "line up " tools to position your text later.
Click the text to be engraved so it is highlighted, go to the "toolpaths tab" (bottom left)
and select the engraving symbol(looks like letter EA)
Set the options for finish depth (0.05mm say), "add" a tool from your tool database( I use a 3mm dia 30 degree engraving bit).
You may have to define your tool to suit what you are using.
"setup" your material for thickness and to say that your Z zero position is on top of the material.
Click "now" and the cnc toolpath is created.
Go to menu/toolpaths/save toolpath as, and in the left window should be the toolpath you just created.
CLick the arrow to copy it to the right window.
From the lower right drop down box you can select your cnc machine if it is listed. If not then select G-code(mm)(*.tap) as this is a fairly generic gcode file.
Click save and save it to your directory of choice.
This is now the gcode file to send to your cnc machine. You can simply change the ".tap" extension to .cnc or whatever your cnc machine expects. ALL gcode files are text files.
Check the file first as it is a simple text file you can read in notepad etc.
When you test it on your cnc machine set a false z 0 point up away from the table with no tool in and run the prog to see what happens. If it does not work as expected then choose a different machine from the drop down box.
hope this helps
regards
geoff

[johnnyg]

Thanks for your reply.When i go to open the attached file it says invalid DWG version and wont open. What could be causing this? I cant even attach the file anymore. I can attach the PDF file though. What could be wrong with my file NOW?

[johnnyg]

I got the file to finally work saving it as DWG Autocad 2010 and made just a text file to engrave text. Now i get an error message in ArtCAM pro like this when trying to set up smart engraving
( error message- Selection contained open vectors- these will be ignored

next error message


Vector intersections were found in the selection. Please identify and correct using the Vector Doctor. ) What does this mean and how do i correct it.

[jonesthesoftware]

Hi
You have to make the text using Artcam not the Autocad text as I explained before. Only use Autocad to make the full size drawing of the panel you wish to make and place the text in the correct position in Atcam. Artcam can import the outline drawing and you can make toolpaths in Artcam to machine out slots/holes etc.
regards
geoff

[johnnyg]

Thanks i finally got this to work with Autodesk Inventor Professional 2016. I was able to make the tool paths for the lettering after changing the font in autocad 2013 to Futura LT then opened it in Autodesk Inventor Professional 2016.

[paul_planes]

Vector intersections were found in the selection. Please identify and correct using the Vector Doctor. ) What does this mean and how do i correct it.

Use the Vector | Vector Doctor tool. It can identify self-intersections and remove them. Intersecting vectors produce bad results when engraving text.

cheers
Paul