running toolpath on an stl

smallshop · Oct 5, 2006

Does any one know which cam systems will run 2.5 and 3d toolpaths on and stl file? I tried it with VisualMill and had no problems. Is it a misconception that most cam packages won't cut an stl file? We get questions from potential customers interested in buying the Nextengine 3d scanner about this and one individual posted on a blog about it being a "non machinable file". RhinoCam seems to be able to do almost as much with a mesh as a nurbs surface. I haven't tried everything but I'm not seeing the problem.I would think most cam packages are the same here? If you know specifically that your cam package will cut an stl file or what the limitations are please reply.

Thanks,

Ted

SAIPEM · Oct 5, 2006

All the mid-range and bargain 3-D CAM systems are generating toolpaths based on tesellations of the surface or solid geometry.
This includes PowerMill, Mastercam, Surfcam, VisualMill, OneCNC, Gibbs and others.

A tesellation is simply a triangulated mesh.
An STL file is simply a different method for defining the mesh data.

VX has the ability to chose toolpathing based on either direct surface data or tesellation.

Generally, if a CAM system can machine 3D Solids or surfaces then it should have the option for STL machining.

A good but cheap, basic STL machining package is MillWizard from Delcam.
It doesn't have all the bells and whistles but it does everything you'd need for prototype or model making.

smallshop · Oct 5, 2006

Thanks Saipem,

I wonder if the fact that stl's are a hassle to do much with in a cad package is carrying over to the cam tools as a false assumption? I would be interested to hear any specific stories of jobs where guys had to cut an stl file.I remember recently someone saying they could cut an stl in OneCne by making a simple planar surface under the mesh. Correct?

All responses appreciated.

Ted

Edster · Oct 5, 2006

I cut an STL in OneCNC. I made a model and set the stl inside of it. Cut perfectly.

BobWarfield · Oct 5, 2006

It is easy to cut an STL file, but hard to modify it in a very friendly way in a CAD package. As SAIPEM states, it is triangulated mesh, so you've lost all the smooth curve and surface information and are approximating that using a mesh.

CAM doesn't care as in most cases its just following the arbitrary path with its own series of arcs and lines to approximate a toolpath on the curve.

smallshop · Oct 5, 2006

So 3d machining would probably be easier than 2d on an stl because you wouldn't have to work at trying to get a wire frame built to run 2d paths on?

SAIPEM · Oct 5, 2006

You wouldn't want to use an STL for 2d Machining.

STL or StereoLithography is desgined for 3D.

smallshop · Oct 5, 2006

Let's make the straw man this: You have an scanned file of your typical mechanical 2d/3d design.Steps, pockets, counterbore, holes, and also freeform shapes. All you have is an stl file. How are you going to cut the part?

I know how to tackle this in RhinoCam. I'm trying to dertimine if this would be a major hassle in other cam packages or if some of the gripes are merely a knowledge deficit on the programmer end of things.

I understand that working on an stl will be more work for me than using an iges file.But in the interest of getting a prototype finished it would still be way less work than making a designer convert the files to what I like to cam on. I can construct necessary geometry to do my 2d stuff pretty easily in Rhino. So if the goal was a quick prototype off a scanned object that had been modified with some modelling clay....no problem. The machining work would be a bit more but the total work would be much less.

Is RhinoCam easier than other cam tools for this specifically? Are all of them pretty much the same?

Ted

Fidel · Oct 6, 2006

Hi Ted,

I almost exclusively use STL files for machining molds using Visual Mill. Check out a story Modern Machine Shop ran about my shop

http://www.mmsonline.com/articles/0500bp5.html

I also use Magics software from Materialise to manipulate my STL files. I normally get an IGES file from my customers - use Magics to create the stl file using 0.0002 inh tolerance. Magics also allows me to create parting lines and also parting surfaces. Never work with scans but Magics has some functions to smooth scans etc. Might be worth a look if you are using scans a lot.

I can use the STL files for 2D work also. Visual Mill has an extract edge funciton that gets edges of pockets etc which can use for 2-1/2 axis pocketing.

Edser wrote
----------------------
I cut an STL in OneCNC. I made a model and set the stl inside of it. Cut perfectly.
-------------------------
Why do you need to set the STL inside of the model? What do you mean by this? Why can't you machine the STL file directly?

smallshop · Oct 6, 2006

Fidel,

Nice article. It's interesting that you actually prefer stl. I have only had to work on an stl file few times and had no problems in visual mill using the same method you just described.Of course the 3d is simple and the 2d just a bit more work.

I'm the design Studio Manager for NextEngine and now that we are selling our latest product we have been receiving questions from end users about which cam packages they can use with our file output. Since the scanner exports a pretty nice stl I think they would have no problems. But I honestly don't know if all cam packages will easily handle stl files or not.Since I have cam experience I'm the go to guy on this question. Which of course means that I kick it over to all you guys...

cadaddict · Oct 6, 2006

I also use Magics software from Materialise to manipulate my STL files. I normally get an IGES file from my customers - use Magics to create the stl file using 0.0002 inh tolerance. Magics also allows me to create parting lines and also parting surfaces. Never work with scans but Magics has some functions to smooth scans etc. Might be worth a look if you are using scans a lot.

Very interesting post Fidel - thanks !!

Paul

wesg · Oct 6, 2006

Surfcam doesn't import stl AFAIK. So you'd need an intermediate step to convert to IGES or whatever.

WatchUrStep · Oct 6, 2006

Does anyone know what size limitations exist within Visual Mill for STL files?

I have exported STL to Rhino and tried the MeshToNurb command, but Rhino worked on it for three hours and then choked.

My typical export size is .05", but the file size ranges from 70MB to 170MB.

SAIPEM · Oct 6, 2006

When you have files that big, switch to the STL binary format.

WatchUrStep · Oct 6, 2006

That is the format I use.

My question is: is there a size limit to the STL files within VisualMill?

I have sent some files to a friend using VisualMill, but he could not get it open. That is why I tried to use Rhino to reduce the amount of data (MeshToNurb). The only way he could open the file was if I exported the file with a coarse subsurface, which made the model look like crap.

chmillman · Oct 6, 2006

WatchUrStep -

I don't understand what you are trying to do here. MeshToNurb in Rhino converts *each and every* facet in a mesh to a single planar NURBS surface. the result will probably multipy your file size by at least 10X, maybe as much as 50X. So if you're starting out with a mesh model of 70-170 Mb, if you try MeshToNurb, you're obviously going to crash, as you're going to run out of memory.

When you say your export size is .05", what exactly does that mean? Chordal deviation? Max edge length?

What are you exporting? 70 to 170 Mb is a pretty big file, perhaps unnecessarily large. Do you have surfaces? If so why are you sending STL's? (meshes).

Wesg - I'm not sure that converting an STL into an IGES will help you with Surfcam - first, I'm not sure IGES supports meshes, and second, even if you did get one into Surfcam, I don't think you can do anything with it anyway, I don't believe you can toolpath on meshes. --ch

chmillman · Oct 6, 2006

OK, you can export polygon data via IGES under a certain specific condition - the following page explains it and has some interesting reading as well...

http://www.okino.com/conv/exp_iges.htm

--ch

wesg · Oct 6, 2006

Quick test, hopefully not significant. Export stl from Pro-E, default parameters. File size 94k. Import to Solidworks ... ugly faceted part. Try to transfer to Surfcam, crashes Solidworks repeatedly.

We've got Nugraf from Okino. I'll have to play with that later.

WatchUrStep · Oct 6, 2006

OK. I am exporting a human skull that is modeled as a Mesh. In the system I am using, which is Blender3D, the only export option I have to a lot of CAM systems is STL (binary only).

In order to get a decent model into my friends VisualMill, I have to reduce my subsurface division to 2, this is the number of surfaces(or triangles)that are created for every vertex on the model. This causes major facets in the model, which renders it useless. I prefer to export with 6 subsurfaces so that the model has smooth transitions and limited faceting.

Now mind you, the file with 2 subsurfaces is about 40MB and the file 6 subsurfaces is about 120MB. Both of these exports provide a model that is .05" from the lower mandible to the crest of the skull. Either way, I just want to know if there is a file size that I should stay within, that way I can save the files accordingly.

thank you all for your assistance.

smallshop · Oct 7, 2006

Now mind you, the file with 2 subsurfaces is about 40MB and the file 6 subsurfaces is about 120MB.

Does anyone know if Rhino 4.0 will be able to handle a file this size? My understanding was that it was improved in this area. If so, RhinoCam pro might be the way to cut on a mesh like this.

running toolpath on an stl

Diamond

Cast Iron

Diamond

Diamond

Hot Rolled

Diamond

Cast Iron

Diamond

Plastic

Diamond

Aluminum

Titanium

Aluminum

Cast Iron

Aluminum

Aluminum

Aluminum

Titanium

Aluminum

Diamond

Similar threads