Hi all.
I'm starting out in solidworks and I plan to make an arcade machine, for that I drew the plans to have them machined by a carpenter who has a CNC.
The carpenter tells me that I didn't use the right tools for my drawing and that unfortunately he can't do the machining with the plans as is.
Can you help me correct them please
Thank you in advance.
Hello
To do this, we should see your assembly as well as your parts to be able to help you.
I can't open your file because you need to have an Sw version after 2016. A colleague will look with a newer version.
No worries and thank you very much for helping me because I really don't know how to do it, if you want the other files I could send them to you.
Good evening
A few screenshots would be welcome so that everyone can see your project
A+
I presume that the problem comes from the type of file that the carpenter needs for his machine. The operation is similar to milling, so in 3D. A simple DWG DXF would therefore not be enough.
What type of file does it need?
I'm far from being an expert, but the play doesn't look bad to me
Hello
He asked me for the DXF format files, he offered me to make the changes himself but I prefer to do it myself and learn at the same time.
He told me that I had to use a polyline tool because from what he told me the milling software does not recognize the lines.
For the record, he would have modified it using autocad
Hello@pierrecolin056
I think your machinist has two remarks:
- it needs DXF (or DWG) file
- I imagine that your part will be made by milling? It is therefore necessary to make milling radii in sharp corners. because it is impossible to realize as it is drawn.
I was also thinking about the problem of strawberry combs.
Another possible problem, which you won't be able to do anything about, is when converting SW-DXF, SW generates lines that overlap and/or are non-joint. As a result, you have to start again after the fact, depending on the software that deals with it afterwards.
Hello
We machine wooden crates and not proceed as follows.
- flattening of the parts in the drawing.
- conversion of parts to DWG (for our part)
- Manual nesting of parts to match a panel format.
- Then we go under the machining software that will generate the CNC program.
In this software (Alphacam for us) allows you to remove common lines, assemble the lines together to make a tool path.
Ideally use arcs and lines and avoid spline curves which avoids arcs too small for digital in some cases.
As for the tool radii, normally it's not a problem, the software has to compensate and leave an arc where you drew a sharp angle. After this arc can be reduced by a milling cutter of a smaller diameter or ground by hand if it really bothers. (in the case of an interlocking for example)
As for the depths and the file type, just a 2D is enough as long as you don't use 5axes. The depth must be provided to the machinist /programmer. For example, the depth of the connecting grooves or the depth of the decorations.
Hope to have given some leads.
I looked at your 1st piece with the PAC MAN, your carpenter will have to use at least a 2mm drill bit to have something correct or an engraving drill bit that will give a better result unless you really need the "hollow" to paint the other one.
Hello
Thank you all for your answers.
I don't really know what to do to solve my problem and succeed in having the different parts machined.
I made my different pieces using the tools to make lines, circles in 3pts, rectangles... (I have the impression that this is what causes him problems.).
then I put it in 3D using a boss function and using the same tools I drew what I wanted to have engraved and with an extrusion function set to 2mm I modeled the engravings on my drawing.
To answer FUZ3D's question I want to paint the engravings next.
By the way , FUZ3D, would you be able to produce what I want from these plans without modifications?
For me I don't see where it is blocking outside the tool shelves.
I could do it but in V-engraving. otherwise you need a wick 1 - 2 mm. (we don't go below 10mm for example for wood and 6mm for foam)
So either he doesn't have the right file (DXF or DWG in 2D) or he doesn't have the computer tools to assemble the different toolpaths (but I doubt it) or he doesn't have the physical tools on his CNC (diameter too big)
Or it does... to do so (which is not excluded... but that's another story)
I think I have done all the possible problems but find which one is the right one.
So here's what it looks like, at first in fact an engraving and at the very end by making a pocket like on the 3D (by cheating on a scale of 2 having a strand of 6 at the smallest to simulate a 3mm strand).
Available as an attachment.
So the very 1st shows in brown that some letters are in curve and not in arc but it's my machining software that can convert them for me.
In 2 the tool paths in engraving. (nothing special, everything is fine)
In 3 the simulation of machining. Everything is fine too.
In 4 is the simulation in 3mm cutter on a scale of 1. And there we can see the finishing problems due to its radius. I didn't make the letters because there is not enough space for the cutter to pass through (ideally 1mm which can be a problem for the carpenter for example)
So in summary the DXF suits me very well, just some curved conversion in arc of a circle but for me it's classic doing a lot of logo engraving. On the other hand, if you want a machining like 3d with 2mm deep grooves in order to paint them, there may be a problem with the tools.
Hello
I agree with everything that has already been said (SW2018 version a priori). If you provide a DXF (or DWG) to the carpenter, I have a few remarks:
1- The engravings will be machined in pocket recesses with a tool (milling cutter or other) with a diameter less than or equal to the minimum value of your engravings because there are wider shapes. Generally on CNCs, the tool's path is shifted by the value of the tool's radius and the closed sharp corners are automatically replaced by the shape of the tool.
2- On the other hand, we can see on the outer contours of the A and the M that there are small segments of 0.24mm and there the CNC will make a mistake. Maybe that's why the carpenter told you that his CNC couldn't accept your DXF (?).
3- I think that switching to polylines (splines) for the curved parts will pose a problem for the CNC because it is possible that:
- Or the CNC does not know how to interpret splines.
- Or, if it accepts them, some splines may contain radii of curvatures smaller than the radius of the tool.
Rounded shapes should be able to be easily replaced by tangent arcs or circles for the letters O and C in your text as well as for "PackMan" shapes.
Kind regards