Hey Folks!
So, I have this model, see... (shades of bad movies)

Seriously though, I'm new to sprutcam, their website is down, and I'm trying to make it do something useful. I think I have most of what I want done, and now I'm trying to get it to "part off" the final part.
I have a 3d model from Alibre, import it as iges, and setup the 4th axis along the y-axis. This let me turn the model all around the axis and mill every side but both ends of the y-axis.
I'd really like to mill off the end face, and then the mounting face as my final steps, but I can't seem to get the software to realize I actually want it to do that. Seems like a simple line, full depth would do it, but I can't seem to figure it out.
Any kind soul out there with hints and tips / tell me how to do it?

Thanks!
Jason

Hi Jason, it's kinda difficult to advise you without seeing the project that you are working on, but, if it is what I think you are trying to do, I would:

Select 2D Geometry mode
make sure 'Snap to 3D model' is turned on
Create a line which will be the edge you want to cut by snapping to the appropriate parts of the Alibre model
In Machining, select 2D Contouring and use the 'Line' you've just created as the Model


Don't forget with 2D Contouring you will have to enter the Top and Bottom levels for machining, and also be careful about whether the cutter is on the left - right or centre of the contour with Compensation turned on/off as required.
If you aren't sure about how to set any of these last things, double click the curve (Line) that you are using in the Model list and you can set them all from the window that opens.

HTH

Dave

Hi Jason, it's kinda difficult to advise you without seeing the project that you are working on, but, if it is what I think you are trying to do, I would:

Dave

Dave, that helps a great deal, thanks! With a little playing around I was able to get everything satisfactory, with one more problem.. :rolleyes:
I use a 1/16" bit, and want to make a 1/16" inch hole... best I can do, is get the countersink around it, but I haven't found the magic that will actually make a hole that size. When I select "drill", it puts a white "i" around it, but will not actually make the path do do it....

Any magical advise for that one?

I really appreciate your time... I've been spending the last few days solid learning first Alibre (cool software!) and now Sprutcam (the manual could be better: where/what/how do you specify options for the holder? And why won't it save from tool to tool? :drowning:

If you're really bored, I can put my .stc file up on my website for you to laugh at.. :}

Thanks!

Jason

Jason, not sure about the drilling problem, if you can put your *.stc up so that I can download it I'll be happy to take a look for you.
I agree with you about the manual, but it's much better now than when I first started using SprutCAM!
The tool holder information is entered on the Tool tab. You enter the dimensions as a series of X & Y coordinates separated with a semicolon:
0.47;1.57;2.16;0;2.36;0.09;2.36;2.36;5.11;0;5.11;0.78;3.34;0;1.18;7.87
You cannot store the tool holder information in the tool library (yet), but what I do is save the holder description in a seperate text file and copy and paste it from there.
Try it, copy and paste the above 'string' into the Holder dialogue......

I never laugh at people who have the courage to give it a go........

Dave

Jason, not sure about the drilling problem, if you can put your *.stc up so that I can download it I'll be happy to take a look for you.

Great! Time for a laugh.. :stickpoke You can find the file at
http://www.txt.com/jason/sprutcam/back.stc

Please remember to put the coffee cup down before viewing; I'm not responsible for you dopping your coffee on your keyboard from mirth!

The tool holder information is entered on the Tool tab. You enter the dimensions as a series of X & Y coordinates separated with a semicolon:
0.47;1.57;2.16;0;2.36;0.09;2.36;2.36;5.11;0;5.11;0.78;3.34;0;1.18;7.87

From playing with the format, it looks like it's 3 dimensions? When I try entering a few things, it does not act quite like I'm expecting... Basically, I'd like to model an ERC20 tool holder for my bits, since that's what I'll be using on my mill.
Maybe what is needed is a couple of things: a tool holder library, so you can save off tool holders, and something a little more intuitive about designing/entering parameters for one? :p

Thanks for the help!

I never laugh at people who have the courage to give it a go........

Dave

Maybe not *at*, how about *with*? :p

Ciao!
Jason

Jason, I'm well impressed! you are doing really well mate....:cheers:

I agree with you entirely about the toolholder issue, it isn't very intuative and I have already asked for holders to be added to the database.......I think that the software guys are flat out on getting the lathe ops done.....hopefully they'll be improving the mill tool library afterwards.
The coordinates are 2 dimensions. Try this, create a 0.5" diameter cylindrical mill, to describe the first part of the holder which is lets say 2" wide by 1" high, first type 2;0 (2 is the width, 0 is the start height), you will see a line appear at the top of the tool, now type ;2;1, you will now see a rectangle at the top of the tool 2" wide and 1" high.......HTH

When drilling holes from a surface/solid model you first need to get SprutCAM to 'Recognise' the holes.
It is a bit hidden away but when you select a Hole Machining operation, click on the 'Holes' option (below Machine - Workpiece - Restrictions) and a little icon will appear, click this and the rest should be fairly obvious :p

You can download your modified project here (www.download.sprut.co.uk/back_dpmod.stc)

Dave

Jason, not sure about the drilling problem, if you can put your *.stc up so that I can download it I'll be happy to take a look for you.

Dave

Here is an example of something I'm finding very frustrating... Maybe a quick look can tell me what I'm doing wrong?

http://www.txt.com/jason/sprutcam/backbad.stc

Basically, I select all of the flats on one side, and do a rough cut on it to clear out most of the stock. When it calc's the path, I find that the paths are going through both sides (where there is suposed to be metal!) and down both sides, when I just wanted the flats and the inside done instead...
I've played with restricting some/all faces that aren't supposed to be touched, it does anyway....

Sigh.

Thanks for any insights...

Whoa! Just saw your reply to my other post, thanks for the fast response, and I'll go look at it!

Jason

Jason, I'm well impressed! you are doing really well mate....:cheers:


Thanks! I'm learning, one frustration at a time. :p

Actually, I think I figured out my last problem.. I have to select EVERYTHING that is not supposed to be in it, not just the majority of the faces... I did that almost by accident, and tried it again, and... and... it's not milling through the metal anymore. (okay, it's missing some of it, but hey.. that's an improvement!)

So, thank you very much for your time and effort, it is much appreciated... I'm getting less frustrated with it (well, except when it crashes!) and I'll probably end up keeping it now (as opposed to going with something else).

Again, thank you very much for your time!


Jason

No problem, last one for today though....it's getting late over here and I desperately need my beauty sleep :p

You can download your corrected project here (http://www.download.sprut.co.uk/backbad_dpmodgood.stc)

To see where you were going wrong you need to understand that the Waterline roughing operation only actually machines the workpiece.......
You can see this if you run SprutCAM, don't import a model but go and create a Waterline roughing operation. Click on Workpiece, select 'Box - from centre point', enter LX 10 LY 5 LZ -2 and now click run, you will see that a toolpath is calculated to machine it all away.

Ok, now if we add a model into the equation then SprutCAM machines the workpiece, but avoids the model.
Because you had selected only a few faces as your model for machining, and SprutCAM calculated a workpiece based on the extremeties of the faces you had selected (Blue wireframe) it tried to machine all of the workpiece less your selected faces.

As you will see in the modified project I have added the whole model in for machining and I have used a curve restriction to keep the machining inside the cavities.
I created the curve for the restriction by using the 'Project' function (3D Model).

Dave

Just a quick afterthought. If you are selecting specific faces for machining, then put the whole model in as a restriction!
This is real belt and braces approach..........but it works and avoids any nasty errors especially if you forget to select a face that is required for machining (which leaves a hole in the model).

Dave

Just a quick afterthought. If you are selecting specific faces for machining, then put the whole model in as a restriction!
This is real belt and braces approach..........but it works and avoids any nasty errors especially if you forget to select a face that is required for machining (which leaves a hole in the model).

Dave
Yes, well, that's how I started, and kept getting "nothing". :p Ah well... I'm slowly getting there. Took me awhile to find out to create curves (You know, the manual just say's "you can do this", but doesn't show how!), because I *know* you didn't hand draw those! But, find them I did...

I managed to get my first (clumsy) model to path everything, and in the order I wanted them, so far... I have a few "tool impacts model at rapid speed", I.e., I thiink that means it doesn't have enough clearance when it does rapid moves between things... which is funny, because when you do it one block at a time, it doesn't say that.. .only when you hit "machine all quickly"...


Again, thanks for your help! I'm slowly digging my way through my 'show stoppers' list, and I really appreciate the help! Eventually I'll probably even get to use this on my mill... :p

Ciao!
Jason

These types of errors aren't usually caused by the cutter being too low when doing X/Y rapid moves, it's most likely a rapid Z move down to the part or the simulation is being run out of sequence with the actual machining order.

Lets look at the last problem first. If a part has two operations done on it: Roughing + Finishing, and in Simulation mode I just simulate the Finish operation, there will most likely be a 'Contact with model on rapid feed' error, this is because the Simulator is checking the workpiece model as well as the 'Part' model, and because the roughing operation hasn't been simulated first, the complete workpiece is still there when the finish tool rapids down to start it's work.

If the warnings are occuring when the tool is doing a rapid move down to the part, then it's usually because the 'Safe distance' value (Toolpath) is too small, usually thsi occurs with a spherical or Torus cutter.
A good 'rule of thumb' to avoid these errors is to allow at least the radius on the end of the tool + your safe allowance.
For example (metric), if I am using a 10mm ball nose cutter, I would always allow 6mm as my 'Safe distance' value. This is 5mm (nose radius) + safety distance (1mm).
The reason for this is that a ball nose cutter can cut on it's end OR it's side.

You could also use a 'Safe level' (absolute) value instead to avoid these problems, but this is at the expense of the cutter always feeding down from this Z height which leads to a longer machining time.

You can easily find out where any theoretical collision is occuring by pressing the '!' stop on collision icon in sumlaor mode.

We can also 'optimise the feed' after simulation.............but that's a bit too advanced for now...........

Dave

These types of errors aren't usually caused by the cutter being too low when doing X/Y rapid moves, it's most likely a rapid Z move down to the part or the simulation is being run out of sequence with the actual machining order.

Dave

Thought you were getting your beauty sleep? :stickpoke Don't blame me if you haven't gotten enough! :p

The one I checked before I quit for the night (It's late enough here that I'm thinking a bit slower) had a rapid move (G00) down to a Z-.185, so I would hazard a guess that you're right, I need more clearance.
Nasty software won't keep the metal stock even close to right... every time I have to quit (crashes) I have to go in and re-do the stock to tell it what I have. That apparently also isn't being saved! Sigh.

Ah well... Back to my book... Enough mental power to read, not enough to read documentation... :devious:

Ciao!

Jason

I've had my 8 hours, daren't look in the mirror though...will frighten myself :rolleyes:

You've mentioned a couple of times about crashes, I take it you mean that SprutCAM is tripping up?
This should not be happening (obviously). When do these crashes occur? Can you repeat the error?

The first thing that I would try is turning down the hardware accelaration for your graphics card by a couple of notches and see if that makes a difference.

Dave

I've had my 8 hours, daren't look in the mirror though...will frighten myself :rolleyes:


Know the feeling.. :cool:

You've mentioned a couple of times about crashes, I take it you mean that SprutCAM is tripping up?
This should not be happening (obviously). When do these crashes occur? Can you repeat the error?


All too often. I get a lot of null pointer errors (normal symptom: unable to read from address 0x000000< something small) when trying to copy settings from one to another, like duplicating a roughing setup for a finish setup.
Then I get really wierd things happening when I try to a lot of create/delete operations (because they don't work as I thought).
I'm running on a laptop, with 2gig of ram (ibm highend series) and I'm not running out of ram or swapping. I am running in imperial mode, so who knows.. :p
later today, when I get the chance, I'll see if I can get you a repeatable model/steps/whatever if you want it.

Well, the wife is now up, and I'm off to bed. 3am, early, right?

Ciao!
Jason

If the warnings are occuring when the tool is doing a rapid move down to the part, then it's usually because the 'Safe distance' value (Toolpath) is too small, usually thsi occurs with a spherical or Torus cutter.
A good 'rule of thumb' to avoid these errors is to allow at least the radius on the end of the tool + your safe allowance.

Dave

Okay, so, each time I start up, i have to reset the stock values to something reasonable (i.e, bigger than .00039 square). After looking it over, and then using my stock size as distances, I realized that sprutcam does not seem to be using the stock sizes properly.. or at least, not automatically. So, setting the safe distance, and safe and top fixed all of the red bangs when running it. Sad that I have to do this again each time I crank up the software.
Makes me want to take another look at visualmill... see if they have as many crashes as sprutcam!

I have my first model almost ready now... I can't seem to get it to understand that when I drill holes, I want them sideways... :p I've got three holes I would like to mill out on one end, which is why I switched to the X axis as my 4th rotation axis. But Sprutcam seems to not let me drill with the model rotated? Am I missing something again? I've tried to get the curves function working with that one, but it still wouldn't let me drill them (or mill them)...

Hope you're having a good weekend!

jason

Each time that you start a new operation you have the option of adjusting the 'Stock' value.
You would only normally have a Stock amount on a roughing operation, although you can use it on a Finish operation to make it a semi finish operation.

The 'Stock' value is the thickness of material that you want remaining on the part after an operation is completed.
The material that you are starting with (square?) is defined by the workpiece which you can adjust, SprutCAM will always calculate one automatically for you.

SprutCAM will only drill holes that are parallel to the spindle axis, so once you have applied your 4th axis rotation you should 'Recognise' the holes (see my previous reply).
If it doesn't recognise the holes then make sure you have the 'Search' options set for the size of holes you are looking for (Dmin / Dmax) and if this doesn't work check and make sure that the 4th axis angle is correct.

Good luck with your VisualMill trial.

Dave

Each time that you start a new operation you have the option of adjusting the 'Stock' value.

Option I would like; having it reset to blank stock that is .0039xx by .0039xxx by .0015 is silly... for a piece that is 2x2x.25. The "automatic by piece" is even worse. :} And I'm talking about the workpiece to machine from, i.e., automatic, box, etc... those are the values that constantly reset. I would have expected (when the auto box is checked) to be at least as large as the model I am milling to; instead, I get this miniscule metal in the middle of my design (in sim mode), and I can't help but think that isn't helping the post processor much. I could be wrong; infact, quite often I am, but it would make sense when checking parts limits and tool paths that you have at least a close approximation of the original material to machine from.


SprutCAM will only drill holes that are parallel to the spindle axis, so once you have applied your 4th axis rotation you should 'Recognise' the holes (see my previous reply).

That's what I tried! I managed to get it to recognize that I had three holes there to do, but it wouldn't take the x/y position from the model; insisted on putting them at 0/0 (on the correct plane, anyway!). Muddling around with things this morning, I found that if I renamed "curve1" to "hole1", then it would let me change the x/y values while retaining the fact that it is a hole. But I have to enter the values from my model, manually.. which means I'm still missing something, doesn't it? :}

So far, I'm close, at least in a learning attempt. I've got it milling off what i want, in the order I need (including cutting off last!), now except for the automatic hole in the 270 rotated framework... It did find the correct holes in the 0 rotation framework...

Ah well... still plugging away... :}

Thanks !!

Jason

Sorry, but I feel like I'm a detective here trying to interpret the evidence........

So (Don's his deerstalker hat), if I understand you correctly, the 'Stock' amounts you are talking about are used for the 'Simulator workpiece' and not the Stock for the machining operation?
If this assumption is correct, then this is used for the Simulation only and has no effect at all with the calculation of the toolpaths.
If you are not using a rotary axis then the 'Use the operations workpiece' in simulation mode will work for most instances.
If you are using a rotary axis (axes) I would recommend that you create a surface/solid model of the workpiece and import this into the 'Workpiece' folder, SprutCAM will then use this Workpiece by default for all newly selected machining operations and also for the simulation mode.

For the Holes recognise function to work correctly, you must have the model (with holes) in the Model list for the Hole Machining strategy, otherwise it will find no holes.
If this isn't the problem then can you make the project available for download or post some pictures up as I need some more clues Watson (takes a sip of Whisky).

Dave

Sorry, but I feel like I'm a detective here trying to interpret the evidence........

So (Don's his deerstalker hat),


As you say sir! As you say... (pulls out notepad) According to our records, the item in question was last seen at http://www.txt.com/jason/sprutcam/backx.stc

And the material it would be milled from is a 2"x2"x.25" block, mounted on a fourth axis along the X axis... Sorta sorry for the imperial measurments. :o

And I think I owe you at least that glass, if not a whole case at this point.
You are correct, my usage of the word "stock" is/was in lines with "I keep blank bars of that size in stock", so meaning what I would machine the part from. As you have probably guessed, I am not a machinest by trade, but infact a programmer, who happens to have way to many hobbies and is now in pursuit of a degree in robotics. And never being the idle one, I see no reason not to make my own robotic parts. :} I've had a Taig cnc mill for years, but no 3d software, so I've done all my drawing in turbocad, then converted and wrote the g-code by hand to mill out the parts. Now I'm upgrading to a Tormach mill, Alibre design software and Sprutcam (so far). So I appologize if my approaches seem wierd or stupid, I'm self taught! What can I say! My teacher didn't know what he was doing! :violin:


If this assumption is correct, then this is used for the Simulation only and has no effect at all with the calculation of the toolpaths.


Ah, good, I thought it did, and was perturbed by it, as I thought the red '!'s were comming from that component of the model. Reassuring to know it's not!


If you are using a rotary axis (axes) I would recommend that you create a surface/solid model of the workpiece and import this into the 'Workpiece' folder, SprutCAM will then use this Workpiece by default for all newly selected machining operations and also for the simulation mode.

Well, I'm sad to say that it doesn't always work, since this part is modeled in Alibre Expert, and imported into Sprutcam...


For the Holes recognise function to work correctly, you must have the model (with holes) in the Model list for the Hole Machining strategy, otherwise it will find no holes.
If this isn't the problem then can you make the project available for download or post some pictures up as I need some more clues Watson (takes a sip of Whisky).
Dave

Let me know where to send that bottle... or will customs drink it while "testing" it for bomb residue? :cheers:

Ciao!

Jason

To get a separate part model and workpiece model from Alibre you can export the models individually from Alibre as IGES models instead of using the SprutCAM shortcut.........
You then run SprutCAM manually and 'Import' the models into their respective folders.......
A little less slick than using the shortcut.........but a small price to pay for the better results when using a Rotary axis.

It appears that the failure to recognise the holes is a tolerance problem. When you 'Recognize' the holes, try using the following values:

Dmin 0.01
Dmax 1.00
Tolerance 0.001

Using Imperial units the tolerance value is defaulting to 0 (zero) which is not helping matters because in Metric it defaults to 0.02.
I have e-mailed the software engineers and have asked them to modify this for future releases (builds).

Well, that's that case solved, "elementary my dear Watson......."

Sherlock.

To get a separate part model and workpiece model from Alibre you can export the models individually from Alibre as IGES models instead of using the SprutCAM shortcut.........


That's actually what I did, exported it to an .igs file, which I can then save elsewhere, and then do the work on that. :cool:



It appears that the failure to recognise the holes is a tolerance problem. When you 'Recognize' the holes, try using the following values:


Yup, that was it... Silly me... thinking defaults came from the tool selected to do the job! :rolleyes:

Thank you very much, that indeed is what was missing. I now know a bit more, and shouldn't suffer the same problems again (we can hope, anyway! My memory isn't... what was I saying?)


I have e-mailed the software engineers and have asked them to modify this for future releases (builds).

Yaay! Wonder if we can get them to fix the null pointer problems... :p

Thank you very much, You have helped this newbie sail the waters of a new powerful tool. Now I'm off to my next project (a somewhat simpler box for a testing device) before I tackle some of my harder projects. But first, I get to learn Motion analysis, so I can do some analyzing before I do machining...
Fun, hmm?

Overall, I am impressed with the tool. It seems to have the abilities to do things I want to do, once I figure out why it's not doing it. If I seem like I have too many frustrations with certain aspects of it, such as the crashing and other programming errors, they stem from me being a programmer, and knowing there are numerous tools to prevent a lot of these simple types of problems if we would use them. More often, we are told to turn off warnings and just get the work done, when a warning is often letting you know of something, that while not stopping the compile now, will clobber you later.

So, again, I'm impressed, and appreciate the help!

Ciao! :wave:

Jason

But first, I get to learn Motion analysis, so I can do some analyzing before I do machining...
Fun, hmm?

Jason

I'm just doing my first bit of motion analysis of the evening, pouring a nice cool beer from the bottle into my glass............:cheers:

Have fun.

Dave

Using Imperial units the tolerance value is defaulting to 0 (zero) which is not helping matters because in Metric it defaults to 0.02.
I have e-mailed the software engineers and have asked them to modify this for future releases (builds).



Just a quick update to the Tolerance problem when recognising holes using Imperial values.
I have received a reply from the software engineers at Sprut, and they say they have solved this problem in the next build.
As a workaround while we wait for this new build they have created a new 'Imperial.xml' which you can download here (http://www.download.sprut.co.uk/imperial.zip).
Unzip the file to your "C:\Program Files\SPRUT Technology\SprutCAM 40" folder and the next time you run SprutCAM this new file will take effect.

HTH

Dave

Just a quick update to the Tolerance problem when recognising holes using Imperial values.
I have received a reply from the software engineers at Sprut, and they say they have solved this problem in the next build.

Hey, that's great!! Thanks!

As a workaround while we wait for this new build they have created a new 'Imperial.xml' which you can download ... and the next time you run SprutCAM this new file will take effect.

HTH

Dave

Way Cool! I've downloaded it, and will give it a try later tonight (rather busy, sigh). Thank you very much!

Jason

Okay, here is a problem I've run into several times... and don't know how to fix it. I've posted the model (one you previously worked on!) with an example of what I'm talking about...

http://www.txt.com/jason/sprutcam/back.stc

basically, I just want to polish off the surface of the model, so I selected finish flatland... I selected the two surfaces I wanted, put the rest into restricted, and... and... wierdness. It skipped one of the surfaces entirely, and part of the other surface wasn't done right. The rest of it was... (oh yes, only the last operation is in question)

What did I do wrong this time? Because I've seen this many times, and don't know what is causing it...

Thanks!

Jason