Printable Version of Topic

Click here to view this topic in its original format

SprutCAM forum _ SprutCAM 7 _ New User: Trouble Generating Toolpaths

Posted by: RamLab Apr 8 2012, 03:20 PM

I have been CNC machining for a number of years using mostly different versions of MasterCAM. I recently started learning SprutCam for the lab I work in.

I found the tutorial videos produced by Tormach and believe I understand the program fairly well. However, after assigning geometry and cutting parameters, when I attempt to generate toolpaths using the "Run" button nothing happens.

I even went so far as to copy the procedures shown in the tutorial videos step by step using similar parts, but it still won't produce toolpaths. It simply says "done".

Is it possible there is some small step I am overlooking? Any help is appreciated and thank you in advance!

Posted by: Sprut_UK Apr 8 2012, 07:16 PM

Hi Ramlab, and welcome to the SprutCAM forum.

It sounds like you are probably missing a fundamental step somewhere, which is not unusual when learning anything new.

It's very difficult to diagnose the possible cause from your description, but if you can attach your SprutCAM project (*.stc) I'll happily take a look at it for you.

Please zip the project before attaching it as this avoids any possible corruption of the file.


Posted by: RamLab Apr 9 2012, 07:56 AM

Thank you for taking a look at this. The path I have attempted to make is a simple roughing pass. From my past experience I would have used drive surfaces to define this tool path, but what I have seen so far from tutorials suggests SprutCam would handle this better with waterline. What is your opinion? ( 182.42K ) : 27

Posted by: Sprut_UK Apr 9 2012, 08:35 AM

The cutter paths are calculated correctly on my setup (see attached image), so we need to find out what is going wrong for you.
Which Windows version are you using?
I haven't used Mastercam myself so don't know what type of cutter paths are calculated using 'Drive surfaces', but the 'Waterline roughing' (constant Z) is probably the one which I would use for roughing this part.


Posted by: RamLab Apr 10 2012, 05:53 PM

The computer is running Windows 7 Enterprise 32-bit. I also made sure to double check that it wasn't something simple like having "show toolpaths" turned off.

Posted by: Sprut_UK Apr 10 2012, 07:05 PM

Ok. Did you apply full administrator rights to SprutCAM 7 both while installing and running?
Having an administrator account does not confer administrator rights in Vista and 7.
A quick way of doing this is to right click the install file or the shortcut / file to run SprutCAM and select 'Run as administrator'.

Posted by: RamLab Apr 13 2012, 08:24 PM

Running as an administrator worked. It is working now, thank you for your help.

So long as I have your attention I do have a couple other questions I would like to ask.

So far as the difference between drive surface paths and waterline paths (that I am used to): a drive surface path would include a variable z, so the cutter could cut a straight line and follow the z contour of a part. Waterline as you know makes each cut at a constant z. This is less important. The REAL reason why I would use a drive surface is because the program would only code toolpaths for those surfaces selected. Where with the waterline toolpath in SprutCam also cuts surfaces that have not been selected (specifically the nosecone of my piece). I know I could use the fixture features in SprutCam to prevent it from trying to cut that area, but is there a simpler way to restrict toolpaths to only the specific selected surfaces?

My other question is a simple one. I am not familiar with the "scallop" option. I gather that it has something to do with surface finish but have not found any literature on how it works. Could you enlighten me?

Thanks again for all your help!

Posted by: Sprut_UK Apr 14 2012, 09:39 AM

It is not clear from your question whether you are referring to a roughing or finishing operation?

I'll assume that you are referring to a roughing operation.
As a general rule, the roughing operations only machine the workpiece and not the surfaces of the part.
Based on this rule, you can immediately see that we can simply make the workpiece the same as the area that we wish to machine, which is ideal if we are machining a casting or something which has had a previous machining operation.
If you need to rough a specific area of a workpiece, whilst retaining the remainder of the workpiece for machining by a different operation, then you can make use of the Job assignment for selecting either faces or Job zone or restricting zone (or a combination of these).
If you use the drive roughing operation, this operation calculates the toolpaths based upon the outline of the selected faces, and this outline creates a boundary (plan view) for the machining itself.
If you use the waterline roughing operation, this calculates the cutterpath by creating a (Z) section at each level, and this section changes at each level, so it is impossible to create a boundary by selecting a face(s) alone, unless that is, the selected face(s) is contained in an isolated cavity / pocket.
You can see this feature by using the 'Perfume box' model included in the Tutorial folder. Simply import this model, then add the bottom face for one of the cavities into the job assignment.
If you use the 'Job zone' option for the waterline roughing operation, this uses a curve to define the boundary for machining and will do what you need. The curve used should ideally be closed and can be curves generated using 2D geometry or projected curves (Model mode) or edge curves.
A restrict zone is defined using a closed curve and restricts machining from this area.

The scallop feature allows the stepover or stepdown of the cutter to be calculated based upon the height of material that remains between each pass of the tool. This allows for example: surfaces with a fairly shallow angle to be successfully machined using the waterline operations which is only normally good for machining faces that have steep angles.

I hope this helps.


Posted by: RamLab Apr 23 2012, 09:38 PM

All of your advice has been very helpful. Using a job zone worked and I have had success with the program. Thank you for your help.

I was wondering if you could point me toward other resources on how to operate SprutCam. I have been reading my operations manual and haven't found very in depth explanations on how to use some of the more advanced toolpaths such as combine paths. Do you know where I might find more literature or tutorials?

Thanks again.

Posted by: Sprut_UK Apr 25 2012, 04:10 PM

You might want to take a look at some of Eric's video's (from Tormach). He does a few Youtube video's:

If you do a search under SprutCAM on Youtube I think that you should find several more resources available there.


Posted by: RamLab May 4 2012, 08:29 PM

Hello again, I am having a bit of an unexpected issue with the same project I questioned you about earlier. I finished the project weeks ago and have run it many times since. After running it a few times I decided my feed speeds were a little off. I reopened the project and changed the work feed rates. I'm stressing the fact that I changed absolutely nothing but the work feed rates (from 24 ipm to 20 ipm) of the toolpaths using the 1/4" ballmill.

The issue appeared when I reproduced the new paths. SprutCam began producing warnings (tool intersects with model on rapid feed). I isolated where in the program this was occurring and have attempted to trouble shoot, after reading through the NC code (at around line 9000) it clearly rapids from its safe plane down to a short distance above the cutting surface before switching back to G01. During this decent it is along side a vertical face of the part that has already been cut, I believe this is where the error/warning is occurring. I have experimented with lead ins and changing the safe plane and cutting planes and haven't been able to solve it.

If you could shed some light on the matter I would appreciate it. More importantly: Why would the program produce toolpaths that were apparently so different from the originals when all I changed was the work feed rate?

The project file is attached, thanks in advance. ( 1.35MB ) : 23

Posted by: Sprut_UK May 5 2012, 03:57 PM

When using a ballnose cutter for a finish operation I always advise using at least the cutter radius plus the required safety clearance when setting / using 'Safe distance' (Lead in/Lead out).
Safe distance is the incremental distance in Z from cutting position that the tool changes from rapid to feed. A ballnose cutter can cut on the end or side of the tool, hence we allow for this by allowing for the cutter radius. Depending on the steps remaining after the roughing operation this amount still might not be enough and may need to be increased.
You could use 'Safe level' instead. This is the absolute position in Z that the tool changes from rapid to feed. Providing the absolute height you give it is clear of any obstructions, this will always work, but could take quite a bit longer machining time because the cutter will have to feed down to depth.

I used a figure of 0.225" (0.125" + 0.1") for the safe distance in both of the operations showing a collision, and this works ok. Click the '%' button to enable a fixed value (=) to be entered.

I hope this helps.


Powered by Invision Power Board (
© Invision Power Services (