Printable Version of Topic

Click here to view this topic in its original format

SprutCAM forum _ SprutCAM 7 _ "Save Geometry as Form Tool" issue

Posted by: bones288 Feb 3 2013, 07:20 AM

Hello all,

Sprutcam is something like the 5th CAM sw that I've investigated while researching the different programs that are available . . . and so far it's winning (by no small measure either).

I am having one problem though that I can't seem to find a resolution for. I've gone over all the tutorials I could find and have through the 600+ page user manual to no avail.

I'm trying to create a form tool in order to create a dovetail mill.

I've stepped through tutorial #3 from Eric and Sprutcam America (http://www.youtube.com/watch?v=f1tRZI1PINQ).
I draw out the profile in '2D Geometry' but the 'Save geometry as form tool' icon does not highlight.

Is there some option or setting I'm not doing right that is disabling the 'form tool' icon?

Any and all suggestions on this are seriously appreciated.

Brad K

Posted by: bones288 Feb 3 2013, 07:44 AM

Odd and interesting update:

When I go to the 2D form tool and select any one of the three lines that make the sample tool I'm trying to create I can get the 'Save geometry as form tool' to highlight.

If more that one line is selected then the icon will not activate for me. Also, when I click the highlighted icon I get none of the options in the tutorial.

Odd.

 

Posted by: Sprut_UK Feb 3 2013, 07:32 PM

Hi Brad, welcome to the SprutCAM forum.

Having looked at your screengrabs I can see that you seem to be doing everything ok, although you don't need to select any of the geometry (lines / arcs) before clicking the 'Save geometry as form tool' option.

One thing that can have an effect on how both SprutCAM 7 & 8 runs is ensuring that it always has full administrator rights. I've created this short video which shows how to do this if you aren't sure: http://www.download.sprut.co.uk/Forum_videos/Administrator/Administrator.html

Are you running the SprutCAM Express version?

Dave

Posted by: bones288 Feb 5 2013, 04:52 AM



Hello Dave,

Thanks for your input on this issue, however it doesn't appear to have any impact. So far I've just taken the desktop SprutCAM shortcut icon and applied Administrator properties via the Advanced / Properties. I never set this option pre-initial install . . . only after the fact. Do you think reinstalling the program and pre-setting this option may be the resolution?

I'm running the SprutCAM 7 trial version Build 0.7 rev 34761.

Yesterday I was talking to a buddy of mine who is much more knowledgeable about CAD/CAM related technologies and he was trying to sell me on GibCAM.
So far. . . not interested.

Oh, can SprutCAM execute dovetail cuts? I see that a few years ago this wasn't possible but am hopeful that this is now a feature.

(What does 'sprut' mean, anyway?)

Thanks again,
Brad K

Posted by: Sprut_UK Feb 5 2013, 07:51 AM

Hi Brad,

If your installation is running in a different manner to that intended, then it might be worth trying to reinstall with full admin rights.

I'm sorry, I've never heard of Gibcam and cannot offer any support or comparison of this for you.

I'm not sure what you mean about executing dovetail cuts? If you mean can SprutCAM generate cutterpaths for machining a dovetail slot(?), SprutCAM has always been able to produce toolpaths for this type of feature it is a simple '2D Contouring' operation. In some older versions it wasn't possible to simulate a cut taken with a 'shaped' tool, but that was resolved quite some time ago. If this isn't what you mean can you please describe what your requirement is?

I believe that Sprut (Russian) would be something like a 'spoke in a wheel' or a ' tentacle of an octopus', but I might have that incorrect.

If you are in the US then I would suggest contacting SprutCAM America and I'm sure Eric (the creator of the video) will be happy to take a look at your tool creation problem.

I created this video a while back which shows a form cutter being produced and used in SprutCAM 7: http://www.download.sprut.co.uk/Forum_videos/Involute_gear/Involute_gear.html

Dave

Posted by: bones288 Feb 5 2013, 08:42 AM



Dave,

I've found your tutorial to be quite informational and I look forward to attempting a few things that you've gone over in the video when I get up in a few hours (you're correct, west coast US).
I'm simply trying to create for myself a 60 degree dovetail mill which I was hoping to simply find online and download into SprutCAM but the more I couldn't find a way to make my own form tool, the more I wanted to.

If all else fails I'll go back and re-install the program as per your instructions in the first video.

Thanks again,
-Brad K

Posted by: bones288 Feb 6 2013, 02:27 AM

So it appears that a newer version of the trial sw has resolved the issue. Finding an 'undercut' mill option was also a pleasant surprise.

(Only issue now is to figure out why the end mills are leaving a little stock behind when the job zone specifies the entire area.)


Posted by: Sprut_UK Feb 6 2013, 07:30 AM

That is good to hear, thanks for the update. The new installer that was introduced with SprutCAM 8 makes updating the SprutCAM installation very easy.
The 'Undercut mill' tool type is available for all of the 'Contouring' operations as well as the 'Rotary machining' operation.

QUOTE
(Only issue now is to figure out why the end mills are leaving a little stock behind when the job zone specifies the entire area.)


If you prefer to explore / resolve this issue yourself then please post up how you resolved it............if you are completely stuck then feel free to post up your problem SprutCAM project (*.stc) on here.
It's best to zip the project up if you are attaching it to a post on this forum.

Dave

Posted by: bones288 Feb 6 2013, 06:14 PM

Actually, maybe I'll quickly ask to see if what I'm seeing is typical or not (seeing as I can't come to an answer myself):


When I perform a Roughing Plane job assignment on a model I'm working on, the 10mm endmill will always leave a little stock behind on the radial plane of the tool.
The axial will drop right down to the model and leave 0 stock behind but this isn't the case for the radial axis.

I've changed EVERY setting in the Parameters section, of that job assignment, and the only setting that makes any difference is the 'Step Parameter' entries in the 'Strategy' section.
But I'd rather not use Scallop'ing and I'd like to leave the default of 50%. (I actually want 0 stock for this roughing operation.)

I've gotten around this by using 2D Contouring instead of Plane roughing for the vertical walls of the model.

Does Plane roughing, by default, leave a little stock behind on the radial axis of the tool?

Thanks,
Brad K

Posted by: Sprut_UK Feb 6 2013, 09:42 PM

If you post up your project that has the problem it will help to actually visualise the issue. It's very difficult to diagnose what is happening from your description.
I don't use the Plane roughing operation very often myself, but some of my customers who are cutting patterns (in modelboard) do use it very successfully.
If you post the project then we can see if there might be a more suitable operation to use.
Can you also indicate what material you will be cutting the part in?

Dave

Posted by: bones288 Feb 7 2013, 08:17 AM

Hello Dave,

Here's the prj I've been learning with. I'm hoping you can you take a quick look and give a few basic pointers for me to run off and go study?

I'd love to learn how to keep the tool from returning all the way to 'home' when successive job assignments use the same tool on the exact same plane.
Also, I'm not sure what the typical speeds/feeds are for milling through steel or 6061 Al and I'm sure the default values are slowing the entire operation down somewhat.
And the dovetail dimensions were just something I threw together and don't truly reflect a real mill.

This is part 1/7 and is clearly the most difficult, so if I can learn on this model then the others will be cake.

Thanks,
Brad K

PS Hard to tell from small image. . . Ducati?

Posted by: Sprut_UK Feb 7 2013, 04:22 PM

Hi Brad,

You are doing well with that project, you are pretty much there with it.............I'll add a couple of notes that I hope you will find useful:

1: I would definitely use Waterline roughing instead of the Plane roughing for the first operation. Plane roughing calculates the cutterpaths by dividing the model into X passes (by default) stepped over in Y which will leave the 'cusps' of material when used on this type of part. You can reduce these by adjusting the 'Step parameters - Distance' to a smaller value, but this will increase the machining time. Roughing plane is very good for rough machining of shallow 'organic' 3D shapes in soft materials e.g. modelboard etc.
Waterline roughing calculates the cutterpaths by dividing the model into Z steps and will not leave behind any cusps of material unless you use the 'Parallel' option.

2: If you are using an identical tool from one operation to the next you will need to use the same tool number........otherwise, if they have a different tool number, SprutCAM assumes that you are changing the tool and will retract to the toolchange position if one is used (see attached image).

3: You appear to be using an auxiliary operation to index the 4th axis, which works, but, you can simply add the required rotary axis angle to an operation (see attached image).

Yes it is a Ducati S4 Monster which is a beautiful machine........but I no longer own her.........I'm only allowed one big toy at a time now rolleyes.gif


 

Posted by: bones288 Feb 8 2013, 05:51 AM

Hello Dave,

Two more questions when you get time . . .

1) Is there anyway for me to modify the .igs file, outside of SprutCAM, and then re-import it without having to recreate all of the job assignments?

and

2) Is the SprutCAM trial only 1 week?!? The open screen says I have 3 days left (2 in a few hours) but I first downloaded it on Sunday. One week seems a bit severe.

And thanks again for the recommendations they've been a tremendous help!
You know, with every problem that gets discovered and resolved two more are found. Onward and forward, right?

Posted by: Sprut_UK Feb 8 2013, 08:00 AM

Hi Brad,

QUOTE
1) Is there anyway for me to modify the .igs file, outside of SprutCAM, and then re-import it without having to recreate all of the job assignments?


If you are using the 'Import' function to replace an existing model (you must delete it first), as far as I am aware the features (faces / curves) that make up the model are given random identities in SprutCAM, so if the number of faces / curves in the model which replaces the previously used version has changed, then it is unlikely that each feature will have the same identity (Face1 - Face2 etc.).
However, I am not sure if this holds true if your are using one of the SprutCAM (CAD) Addins.
The entities that have been selected in a 'Job assignment' are identified by the identities given at import time, so there is no guarantee that these will carry through to the revised model.

QUOTE
2) Is the SprutCAM trial only 1 week?!? The open screen says I have 3 days left (2 in a few hours) but I first downloaded it on Sunday. One week seems a bit severe.


I don't know what the default trial period is now. It used to be 1 month, but I know that this did change to 2 weeks.............I am unaware of any changes to this.
If you contact your local SprutCAM reseller they should be able to extend your trial period for you. If you have any difficulties with this, send me a PM and I'll see if I can help.

Dave

Posted by: bones288 Feb 8 2013, 10:40 PM

Well, I made the model changes and was able to implement all of the job assignments is relatively short order (5th times a charm and you really do learn better ways of approaching things with each pass).

So I have a new question that has come up in the past but, at the time, other questions took priority:

When using the undercut mill I noticed that, instead of clean sharp lines being in the slot, there was an odd vertical 'ledge' (see image w/ tool settings insert).

Any ideas?


(side note: if I joined the forum on the 1st after having struggled with learning for a few days. . .maybe I have been doing this for 2 weeks!?! Time flies.)

 

Posted by: bones288 Feb 8 2013, 11:43 PM

Apparently scrap that last post. When I push the speed bar all the way to the right and the mills fly though the stock, the dovetails show up correctly.
Looks like it may be a sw issue.

Posted by: Sprut_UK Feb 9 2013, 01:00 AM

Hi Brad,

It's late here, so a quick answer for now:

It looks to me like you don't have the angle of the tool set to the same angle as the (angled) feature being machined.

If you don't know the angle of the face, you should be able to double left click on the angled face (geometry model), and you will be given the angle:



You can then enter this angle in for your Dovemill:



This is an end on view of the simulated machining and the cutter matches the Part:



HTH.

Dave

Posted by: bones288 Feb 9 2013, 02:17 AM

Interesting trick. But the angle in the Geometry model is set to 30 like the tool. Sometimes, when I simulate the operation repeatedly, the slot edges are sharp and other times they'll ave that flat vertical plane. If the model doesn't 'appear' to mill correctly the first time I can redo that step on high speed until it comes out looking right.

It's just a visual thing here and the actual code/paths that would be generated would come out fine every time.

Posted by: Sprut_UK Feb 9 2013, 09:49 AM

Hi Brad,

You're right, it would be very strange if that is the case (wrong angle). Please post up the project used in your previous image and I'll take a look and will pass it on to the software engineers if there is a fault..........if that is acceptable to you?

Dave

Posted by: Sprut_UK Feb 10 2013, 07:25 AM

QUOTE (bones288 @ Feb 9 2013, 02:17 AM) *
Interesting trick. But the angle in the Geometry model is set to 30 like the tool.


I am now wondering whether you have used the excluded angle of the part rather than the included angle. If this is the case then your part might be a 60 degrees in which case the tool should be set to the same value. This can be quickly ascertained when you send your project.

Dave

Posted by: bones288 Feb 11 2013, 04:55 AM

Hello Dave,

I hope your weekend went well. Mine was some what disappointing.
I'm working on prototyping my first parts to prove out the concept for a patent I've submitted (attachment is the official receipt I received as of today).

There are 8 parts that need machining and I decided to learn SprutCAM (models created in Inventor) on the hardest parts first.
Now that I've learned the program enough to get by I find that the trial is only 2 weeks long. sad.gif

In the one day I had left I was able to put together the toolpaths for the 2nd hardest part. A terrific learning curve, in my opinion.
But now I have no more time and no parts to see if there's interest. If there is (and I think there will be) then the simplified prototype, being made now, would need to be recreated into a commercial production model and there would be many more 'lines' created each one needing different machining.

I can't take a chance on a $3500 package, I would need Expert at the very least, until I know if these are going to work and ppl are interested.
Is there anyway to get 2 more weeks out of the trial sw? I'd still need to learn the post-processor part of things which I only just began yesterday.

If this is too much then I completely understand.

Posted by: bones288 Feb 11 2013, 06:13 AM

QUOTE (Sprut_UK @ Feb 9 2013, 11:25 PM) *
I am now wondering whether you have used the excluded angle of the part rather than the included angle. If this is the case then your part might be a 60 degrees in which case the tool should be set to the same value. This can be quickly ascertained when you send your project.

Dave



My appologies. . .I see that I forgot to attach the prj of your request.
Let me know if it acts the same way for you as I can't run the tool paths now that my trial has ended. (I think this was the final prj file for that item.)

Thanks again for all of you help! I really do appreciate it.

(Resent as .zip)

Posted by: Sprut_UK Feb 11 2013, 08:00 AM

Thank you for your project. With regard to the tool it is correctly set in this project.........although it does appear to be a different project to the one shown in your original post about the problem (see attached screengrab).

QUOTE
I don't know what the default trial period is now. It used to be 1 month, but I know that this did change to 2 weeks.............I am unaware of any changes to this.
If you contact your local SprutCAM reseller they should be able to extend your trial period for you. If you have any difficulties with this, send me a http://forums.sprutcam.com/forums/index.php?act=Msg&CODE=4&MID=4 and I'll see if I can help.


Dave

 

Posted by: bones288 Feb 12 2013, 08:11 AM

Dave,

I may have just had a revelation and need your opinion on something.

Can the rs_top.stc file that I sent you earlier be completed with the Machinist package?
From what just dawned on me 2.5D - 4th axis indexed milling is all that is truly required to make my proto parts? And I wouldn't require true 3d milling for that (at this time, anyway).

Is that a correct statement?

Thanks,
Brad

Posted by: Sprut_UK Feb 12 2013, 08:45 AM

Brad,

The Roughing is going to be the main difference. The Machinist version does not include the Waterline or Plane roughing operations.............you will need to use 'Pocketing' or '2.5D pocketing' instead.
The Machinist version includes indexed rotary axis machining so I think that the machining might take a bit longer to prepare using the Machinist version, but it would be possible.
The main difference between the 3X or Expert versions and the Machinist version is that the Machinist version cannot calculate any cutter paths directly from the imported 3D models faces (surfaces).

Dave

Posted by: bones288 Feb 12 2013, 06:47 PM

Dave,

Correct me if I'm wrong, using the Machinist version of the sw I would have to recreate each model using the 2D Geometries vs. simply importing the existing models from elsewhere?

(Losing the two roughing operations, for prototyping purposes, would be okay as cutting time and efficiency are optional at this point. )

Thanks,
Brad K


Posted by: Sprut_UK Feb 12 2013, 08:48 PM

Well it would be better to start a new thread for each topic, it makes it easier for other users to navigate the information.

You can still import a 3D (surface / solid) model, but you can only use the wireframe 'edges' of the imported model in the Machinist version. For the (2D) Pocketing operation you have to select the 2D curves / edges and define them as a 'Boss' or a 'Pocket' and set the top and bottom levels (Z).
In the Machinist version you cannot just import a surface / solid model and start machining it.

HTH

Dave

Posted by: bones288 Feb 13 2013, 09:54 PM

Dave,

Can the machinist version do threading and hole tapping? (I'm assuming so.)
The machinist trial version from Novedge doesn't appear to be working for me at all (no boot) so I can't inspect the individual milling features.
I'd like to be sure that I can tap the holes I drill with this version.

Thanks,
Brad K

Posted by: Sprut_UK Feb 13 2013, 10:00 PM

Hi Brad,

Yes you can do thread milling and tapping with the Machinist version.

I'm not sure what SprutCAM activation method Novedge use for their customers, so you'll need to contact them direct for support with that.

Dave

Powered by Invision Power Board (http://www.invisionboard.com)
© Invision Power Services (http://www.invisionpower.com)