Step-by-step: generate the file, import it into RayTools CutAhead (CypCut) cutting software, set kerf and cut order, then cut.
Your machine The laser is built by Henan Machinery and runs RayTools cutting software — on this machine it is labelled CutAhead on screen, and the same program is also known as CypCut. All these names mean the same RayTools software, so if you see “CutAhead” or “CypCut” anywhere below, that is your program. The steps and button names below match what you see on that screen.
In this app: Everything is millimetres; the file says so in its header.
On the machine: The imported drawing must measure the same as the size shown here. Check one dimension.
In this app: The width × height printed under the preview.
On the machine: Measure the same overall width after importing. If it's out by 25.4×, the units were read as inches.
In this app: Saved on the Machine page. If 'apply kerf' is on, it's already in the file.
On the machine: Then leave compensation off. If it's off here, switch compensation on there with the same number.
In this app: Saved on the Machine page. If 'add lead-in lines' is on, short run-up lines are in the file.
On the machine: Then don't add lead-ins there too. Otherwise set inner and outer lead-ins there instead.
In this app: Shown numbered on the Cut order page: letter holes and mounting holes first, plate outline last.
On the machine: After sorting, confirm the outline is the final cut. If the outline goes first the sign drops before the holes are cut.
In this app: If stencil bridges are switched on, the tabs are already part of the shape.
On the machine: Don't add the software's own bridges or micro-joints on top — you'd get double tabs.
Work down this list at the machine. Each step says what to do, what you should see, and what it means if you don’t. Tick them off as you go — the last column is your record of what worked and what failed.
On the generator choose the “Full address plaque” preset, set the real house number and street, and leave the backing plate on.
Worked if: One solid plate with the letters as holes, and four mounting holes.
Failed if: Letters look spindly or a stroke almost closes up — raise the letter height or pick a heavier font before exporting.
Press “Check cut order” and read the numbered list.
Worked if: Every letter hole and mounting hole is numbered before the plate outline, which is last.
Failed if: Outline is not last — move it down with the arrows and export again.
Download the DXF from the cut-order page onto a stick and open it on the machine.
Worked if: The file opens straight away, no import dialog asking about units.
Failed if: It asks for units, or nothing appears — re-download; do not rescale by hand.
Read the overall width the machine reports.
Worked if: Same number as the width printed under the preview here.
Failed if: Out by about 25 times — the units were read as inches; set the drawing to millimetres and re-check.
Select everything, open Compensate, choose your material entry, set “Expand and contract”.
Worked if: Outline grows slightly outwards, letter holes shrink slightly inwards.
Failed if: You already ticked “apply kerf” on the Machine page here — then skip this step entirely, or the sign comes out twice compensated and the letters go fat.
Letter holes and mounting holes get Inner Cut; the plate outline gets Outer Cut.
Worked if: Every pierce dot sits in waste metal, never on a visible edge.
Failed if: A pierce mark lands on the plate edge — the outline was set to Inner Cut by mistake.
Press Sort, then run the simulation and watch it all the way through.
Worked if: All holes cut first, plate outline traced last, no crossing of an already-cut edge.
Failed if: Outline runs early — sort again or move it manually. Never cut with the outline first.
Cut a single plate in the real material.
Worked if: Clean holes, no slag bridging the thin parts of the letters, plate stays flat.
Failed if: Letters closed up or edges rough — note the material and thickness, then adjust the kerf on the Machine page and cut one more.
Lift the plate off the bed, knock off any dross, wipe it.
Worked if: Finished sign, one piece, nothing to assemble.
Failed if: Plate dropped through the slats — add a MicroJoint on the outline next time.
A DXF file is a plain drawing file that every cutting program understands. The file contains only closed outlines — no text objects, no fills, no colours — which is exactly what a cutting controller wants.
Curves are written as many short straight segments rather than splines. Splines are the usual reason imported letters look lumpy or fail to generate a cut path.
If you turned on a backing plate, the plate outline and the letter holes are all in the file as separate closed contours. If you turned on stencil bridges, the bridge tabs are already cut into the letter geometry. RayTools does not need a special setting for either — it just cuts the shapes.
Tip You can verify the shapes by downloading the SVG and opening it in any browser — what you see is exactly what gets cut.
In RayTools, click File → Open (or the Open button) and select the .dxf file. The drawing arrives already in millimetres, so no scaling step is needed.
After import, RayTools can auto-optimise the graphic — let it. It will merge duplicate lines, join segments, and delete invisible micro-fragments.
Check the reported part size on screen against the width and height shown on the generator page before cutting.
A backing-plate sign is cut from ONE piece of metal. There is nothing to glue, weld, or assemble afterward. The letters are holes cut through the plate — you see the wall behind the sign through the letter shapes, exactly like the signs on design sites.
This is why a 4 or an A is no problem: the little closed middle of the letter is just a small hole in the plate. It stays exactly where it is. Nothing can fall out, because everything is one solid sheet.
The mounting holes are drilled by the laser at the same time. When the cut finishes you take the plate off the bed, and it is done — maybe a quick wipe. That is the whole job.
If you choose "No plate" instead, each letter is cut out as a loose piece you mount individually. In that case turn on stencil bridges so the closed middles stay attached to each letter.
Tip For a first-ever job, always use a backing plate. It is the most forgiving way to cut: one piece, nothing loose, nothing to line up.
A laser beam has a physical width (the kerf), typically 0.1–0.3 mm depending on material and thickness. Without compensation the cut parts come out slightly the wrong size — outer edges shrink and inner holes grow.
Select all the graphics, then click Compensate in the Home sub-page. In the compensation library, pick your material and thickness — RayTools loads the correct Extended Distance and Inside Shrink Distance automatically.
Set Compensation Way to "Expand and contract": outer contours (the plate outline) expand outwards, and inner contours (the letter holes) shrink inwards. This keeps both the plate and the letter cutouts at the right size.
Tip If you don't have a compensation library set up, enter the kerf value manually. For 3 mm mild steel with a 2 kW fiber laser, a typical kerf is 0.15–0.2 mm. Ask your laser supplier for the exact value for your machine and material.
The compensation library is simply a saved list inside RayTools: each entry says "for this material, at this thickness, compensate by this much." You set it up once per material and never think about it again.
Step 1 — get the kerf value. The easiest way is to ask your laser supplier or the machine installer: "What kerf / Extended Distance should I use for 3 mm mild steel?" Write the answer down.
Step 2 — no supplier answer? Measure it yourself. Cut a 50 mm square test piece (type 50 x 50 into any DXF or use a test file). Measure the finished square with a digital caliper. If it measures 49.8 mm, your kerf is 0.2 mm (the amount the beam ate away). Half of that (0.1 mm) is your Extended Distance.
Step 3 — enter it in RayTools. Open the compensation library, add a new entry, name it clearly (e.g. "Mild steel 3mm"), and type in the Extended Distance (half the kerf). RayTools applies the matching Inside Shrink Distance for inner holes.
Step 4 — save it. From now on, for every sign in that material: select all → Compensate → choose "Mild steel 3mm" → done. Two clicks.
Repeat the same once-off setup for each material you stock (e.g. stainless 2mm, mild steel 3mm, aluminium 2mm).
Tip Write the final values on a sticker and put it on the machine. Anyone who walks up to it can then pick the right entry without guessing.
Leadlines let the laser pierce outside the cut path and glide in smoothly, avoiding a burn mark at the start point. RayTools auto-detects inner and outer contours — the plate outline is the outer contour, and the letter holes are inner contours.
Select the letter-hole contours and click Inner Cut — this puts the leadline inside the hole so the pierce mark is hidden in the waste material.
Select the plate outline and click Outer Cut — this puts the leadline outside the plate so the pierce happens in the scrap around the sign.
Click Sort in the Home sub-page to auto-sort the cutting sequence. RayTools will typically cut all inner contours (letter holes) first and the outer contour (plate outline) last.
This matters: if the outer plate is cut first, the piece can shift on the bed before the letters are cut, and they end up in the wrong place. Inner-first keeps the plate rigid while the holes are cut.
Use Simulate (Simu button in the CNC sub-page) to verify the order before cutting. You should see all the letters cut first, then the plate outline traced last.
If you want the finished plate to stay attached to the surrounding sheet after the outer outline is cut (so it doesn't fall through the slats), add a MicroJoint. Click MicroJoint in the Home sub-page and click on the outer contour — RayTools leaves a tiny uncut tab that holds the piece in place.
After cutting, snap the sign free and file the tab flat. This is purely optional — if you have a clean bed or support bars, you can skip it.
Tip RayTools also has its own Bridge feature, but if you already turned on stencil bridges in this tool, do not also add RayTools bridges — you'll get double tabs.
Click Process and select your sheet material and thickness. RayTools loads matching power, speed, frequency, and gas pressure settings from its parameter library.
If you don't have a parameter library set up, enter the values your laser supplier recommends for the material and thickness you're cutting.
Run Simulate one more time to confirm everything looks right, then start the cut.
Thin strokes are the main failure point. As a rule of thumb keep the narrowest part of a letter at least twice the material thickness — in 3 mm steel, aim for 6 mm minimum stroke width. Increase the letter height or pick a heavier font if the preview looks spindly.
Serif fonts with hairline strokes need more height than a heavy sans to survive cutting and handling.
This tool never talks to the laser. The controller has no public interface, and driving a multi-kilowatt fiber laser around its own safety-checked software is not something to attempt. The DXF handoff is how the whole industry works.