Complete newbie here! We have just begun our CNC adventure with a Shapeoko HDM. I am using Carbide Create V7. This has been quite the learning curve but this community has already helped me so very much by reading. I am about to cut my first letters and shapes out and just need advice.
I am attempting to cut out letters and shapes to be put on a round board for a door sign.
First in the design-when creating text I was told to check Convert to Curves but they didn’t really know why. Any explanation on this?
Toolpaths is where it gets tricky.
Using a 1/8” end mill bit - again based on what I have read
I select contour for cutting out letters correct? I mean I am just going on what I have read. I know zero.
If I want to cut out I choose stock bottom.
Is there a certain offset direction to choose?
Then I see the tabs w and h but how do I insert them in?
For my first toolpath I choose the interior parts of letters correct? I tried to put pic but I’m new and only allows one pic.
Then my second toolpath I highlight all things and create a toolpath for it?
When I show simulation the name doesn’t show as cutting out the name completely.
I am sure I am missing something important but that is what I need you guys for. Attaching simulation pic.
You do not necessarily need to convert your text to curves. It depends on the design and if you are trying to do stacked text or other merges with other objects. So if it is just plain text I would not convert them to curves. So if you are just wanting plain text in the font of your choice you have two choices. Pocket or contour. The pocket will remove all of the letter to the depth you specify. With a pocket you have two choices. Simple pocket with a straight bit or Advanced vcarve. The Advanced vcarve has an option to remove the center of the letters with a flat end mill and then use a vee bit to go around the outside of the letters to create a vee shape. This can be attractive and very useful for epoxy or inlay filling of the letters. The second method is the contour cut where you can cut inside, outside or no offset. The contour cut for inside simply cuts around the inside perimeter of the letters. The outside does the same but on the outside edge of the letters. And the no offset goes around the center of the lines of the text.
I often pocket out letters and paint them or fill them with epoxy. The contour can also have the recess filled with paint or epoxy. I dont mean the pocket is literally filled with paint but painted and then the excess on the top surface sanded off. If you are going to paint your object or epoxy it is best to use dewaxed shellac first and then paint. The reason is the shellac keeps the paint from soaking into the grain of the wood surrounding your letters. Also if using epoxy it keeps the same epoxy from soaking into the pours of the wood. I use Zinnser Universal Sanding Sealer (dewaxed shellac) you buy at the big box stores or almost any where. Zinnser also makes a traditional shellac finish but can have wax. The wax can cause adhesion issues with paint, epoxy or top finishes.
You can mask your carves with Adhesive Shelf Paper or oramask. However many times the mask gets torn up on the edges but still limits the clean up of the over spray of paint. I typically use acrylic paint to paint my signs and plaques because it is water based and clean up is easy. I have several brushes but I typically use a 1/4" brush to get down into the crevices of the carving. Some acrylic paint requires two coats. Colors like yellow can look faded after the first coat and may require a second coat to get the pop of yellow. Also the underlying wood like walnut will make the first coat look light. Always let the paint dry completely before recoating or sanding. Wet paint and saw dust do not mix well.
I use MAS table top epoxy with colorants for many vcarve projects. The MAS can go up to 1/4" depth and typically set within 24 hours. If you have deep pours then use a deep pour epoxy but that takes up to a week to completely cure.
This was an advanced vcarve on south american walnut. I used the MAS table top epoxy with Alumite White Resin Dye. I have also used TransTint dyes for other colors. You want to use a colorant that is compatible with epoxy. Most water based colorant is not compatible with epoxy.
This was cut with a 15 degree vee and a 1/32" flat end mill. The sign is 12" X 10". Watco Danish Natural Oil finish was applied. The walnut got considerable darker with the oil finish but the contrast is quite good.
This was cut with the same 15 degree vee bit for the car because the original line drawing had quite fine lines. The lettering was cut with a 60degree vee bit.
This sign was painted but the above was epoxy filled (Williams). So it depends on what you are trying to accomplish which method you do to create a sign or plaque.
Which order one cuts thing depends on what one is trying to achieve — usually strategy is:
delicate details such as V carvings
larger tool first, working from inside → outside, shallow → deep
smaller tools next, REST machining paths, cleaning up pockets and other details
outside contours are last.
Whether or no a cut can be made as a pocket is determined by whether or no the tool will fit — the narrowest passage needs to be about 10% larger than the tool you are using:
Depends on what is currently selected and how one wishes to structure the file:
if all your geometry is on the DEFAULT layer and you have currently selected what you want associated with the toolpath, choose “Use Current Selection”
if all your geometry is on the DEFAULT layer and you do not have currently selected what you want associated with the toolpath, choose “Cancel”
if all your is divided up by layer, and the geometry which you wish to cut is on a particular layer and you intend to only put geometry associated with that toolpath on that layer, choose, “Select by Layer”
Thank you so very much for all the wonderful advice. You know your stuff!
I may not have been clear but I am trying to use the cut outs on a sign. So I would like to use the actual cut out of the name and it just didn’t turn out well. The shapes cut out fine. I love that font and just need to determine the correct settings to achieve the cut out of the name. I may need to make larger.
Only if you need to edit the vectors in any way. If you are cutting the text as-is, no need to convert to curves.
Depends on how much detail you want. Round tools cannot fit into sharp corners. A 1/8" tool will leave a 1/16" radius in any sharp corner, or corner where the radius is less than 1/16".
Contour path traces the vectors you choose. I just cuts along the line, no where else. You can trace inside, outside, or right on the line (No Offset). This is the only path type you can use on open vectors (Pink / Magenta)
Since you want to cut out the letters & keep the letters, you would choose Outside. You can select the whole letter or the whole text, and it will figure out that the inside of the “P, a, l” need to be cut inside rather than outside.
One thing to consider here is the thickness of your stock. With an 1/8" cutter, I would not simply contour anything much thicker than 1/4". When you cut a slot the same width as the cutter, the cutter is “fully engaged”. That is, it’s cutting with the full diameter across the leading edge of the cutter.
As you get deeper with subsequent cuts, chips will get jammed between the tool & material, and can create enough force to exceed the force of your stepper motors to hold the tool in position. This is what’s referred to as “Losing Steps” and when it happens the tool is no longer where the machine thinks it is, and will result in a staggered slot, or multiple depth of cut that don’t line up.
When cutting thicker or harder material, it’s better to offset the vector by the diameter of the tool plus at least 10%. I usually go 25-50%. Then select both the letter & the offset & do a pocket path. Pocket removes all of the material inside the outermost selected vector. And will stop cutting at a nested vector.
Tabs you place on the Design page.
And then decide when you use them & size in the toolpath.
This allows you to do multiple paths using the same tab location.
