parting off a 3d model...

[jasonwinters]

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

[S4 Monster]

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:

1. Select 2D Geometry mode
2. make sure 'Snap to 3D model' is turned on
3. Create a line which will be the edge you want to cut by snapping to the appropriate parts of the Alibre model
4. 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

[jasonwinters]

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..
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?

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

Thanks!

Jason

[S4 Monster]

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

[jasonwinters]

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.. 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?

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*?

Ciao!
Jason

[S4 Monster]

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

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

You can download your modified project here

Dave

[jasonwinters]

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

[jasonwinters]

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

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

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

[S4 Monster]

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

You can download your corrected project here

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

[S4 Monster]

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

[jasonwinters]

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". 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...

Ciao!
Jason

[S4 Monster]

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