[LRF]

I have SC8.
Question, I have a part that gets eventually machined on 2 sides. I write a program that machines the first side complete. I then would like to take the results of that first program, with its remaining machining stock, flip it over and write a whole new program to machine the second side (which is opposite of the first).
Is this possible? I want the second program to be fully aware of the machining that was accomplished by the first program.
Or do I need it all to be part of the same first program as shown in a couple of the tutorials on Youtube? This method is inconvenient when talking in terms production as the 2 side do not use the same methods of clamping in the vise (the vise jaws are different and changed)

[popspipes]

LRF,

I use sprut 7 and I think I do what youre wanting to do. I write a program for one side and machine it, then flip the part and mount to a fixture, indicate it, set zero, and run the second program.

I export the front side of the part from CAD and import into Sprut, and write a program for it.
Next I export the reverse side of the same part from CAD and write a program for that after importing into Sprut.

I post process these files separately and run as side a and next run side b. after flipping the part it needs to be indicated in and the tool height set.

I do this on several of my parts as they have a 3 d hole in them and it cant all be machined from the first side.

[LRF]

Mike,
Thanks for your comment and I also do the same as you on all my products now, however I must not have made myself clear. I want to know if I can export the finished results, from the first SC's programs machining into a new SC program and then write the machining operations for the second side using the results from the first program.

In the first program you usually have your part plus the machining stock which encases the part. After completion of the first program some of the desired features have been machined and some of the original machining stock remains. I would like to use those results as the part model for the second program. That is what I am asking and if yes some coaching on how to would be desired.

Another way of thinking maybe, if you watch one of the SC tutorials on flipping a part, they are writing a single program that firsts machines one side then they flip the part, establish a new set of coordinates for the other side and then continue machining. I wish to do it with 2 separate programs. Currently I write a program for the first side to it completion, then I write a new program but with the part flipped. However in this method when you flip the part it takes time to establish a new machining stock that mimics what is left on the parts after the first machining process and also it doesn't know that possible a hole thru which was drilled in the first program is already done.

[TurboStep]

This is how I machine all my parts:
Select New Operation - Auxiliary - Group. Then put all operations for one side inside this group. Then put all ops for the second side in a second group. Generate the entire project but deselect the second group (double click on the small icon to the right of the group in the ops browser) before calling the post processor. This disables all ops in the group. Gcode will only be generated for enabled groups or operations. Disable the other group and repeat, not forgetting to use a different file name
Step

[popspipes]

Mike,
Thanks for your comment and I also do the same as you on all my products now, however I must not have made myself clear. I want to know if I can export the finished results, from the first SC's programs machining into a new SC program and then write the machining operations for the second side using the results from the first program.

In the first program you usually have your part plus the machining stock which encases the part. After completion of the first program some of the desired features have been machined and some of the original machining stock remains. I would like to use those results as the part model for the second program. That is what I am asking and if yes some coaching on how to would be desired.

Another way of thinking maybe, if you watch one of the SC tutorials on flipping a part, they are writing a single program that firsts machines one side then they flip the part, establish a new set of coordinates for the other side and then continue machining. I wish to do it with 2 separate programs. Currently I write a program for the first side to it completion, then I write a new program but with the part flipped. However in this method when you flip the part it takes time to establish a new machining stock that mimics what is left on the parts after the first machining process and also it doesn't know that possible a hole thru which was drilled in the first program is already done.

I think you are concerned with the machining results from side a, Sprut doesnt care what was done on side a in the side b program. It will only machine the model portions selected in the side b program. If its indicated correctly (as off a thru hole etc) it will machine only what its told to machine in the side b ops and they will match up to side a.

I use g54 for both programs a and b.

The side b on my programs finishes parts of the 3 d holes, counterbores etc started in side a.

[LRF]

Thanks TurboStep, I think you understood the question, and I will investigate your advice. I Like! I'll let you know how I make out.

[LRF]

Mike
Thanks, I understand what you are doing and that is the current way I do 2 sides however looking for a new way and a faster way. I think TurboSteps idea is what I was looking for.

All,
If anyone else has an alternate way please let us know.

[mountaindew]

I do multi sided parts "as many as 6 sides all in one program" with all the code and run it from start to finish and fixtures also . I don't like all the extra files. Also the way I set them up with auxiliary operations that stop the program in places to allow you to flip part set ucs and touch off x,y,z, if required and continue. I can also stop at these points and restart in same place next day if I want and finish the job another day. Path pilot also makes this even more reliable and easy to do after you get the process down.


example of part that has 3 sides
Attachment 285480
Note last operation in list is my favorite


Attachment 285482
The finished part!
As I noted above I can also end the program at end of each group and restart it there the next day or whenever with no problems. No need for lots of extra files.
And of course when you run simulation all results carry from side to side to finished part.
Must note this works best if you avoid using g54 in the program if your using path pilot.

[Jake_Tormach]

Hello all,
There is an option in SprutCAM but it is limited. When in the simulation tab, run your entire simulation. Now right click in the white area below the operations and choose Save Simulation Result. It will save it as a .stl file. Although this is a model file, it's not as crisp as an .igs file and therefore can become difficult to work with at times (faces/edges). It is though very useful for using it as a work piece or stock item. TurboStep has the way I personally would go about it but I just wanted to make sure though that everyone knew you can save the simulation result as a model as well. Good day and I hope everyone had a safe and fun 4th!

Jake from Tormach

[Uman]

This is how I machine all my parts:
Select New Operation - Auxiliary - Group. Then put all operations for one side inside this group. Then put all ops for the second side in a second group. Generate the entire project but deselect the second group (double click on the small icon to the right of the group in the ops browser) before calling the post processor. This disables all ops in the group. Gcode will only be generated for enabled groups or operations. Disable the other group and repeat, not forgetting to use a different file name
Step

This method works. The key is to "Generate/Run the entire project" before deselecting first side group; then deselect first group side and Post Process, otherwise SC is oblivious of previous operations and this most likely will change SC tool path for the second side.

Uman

[wtopace]

Why bother with hacks and workarounds? I just use Sprut's built-in ability to work in multiple coordinate systems and G5x offsets. It's really not very hard and you end up with a single g-code file as well, plus you can simulate end-to-end and watch your part flip in the simulator (make sure you switch the CS at the top and select a pre-defined iso view and it will automatically re-orient).

PathPilot actually requires you to stop and restart the code anyways, you just don't need to load file1, file2, file3, etc...

Here's a newer video that explains coordinate systems pretty well: https://www.youtube.com/watch?v=R7nJ96NOhyI

Learn it, you won't be disappointed.

[mountaindew]

I agree with wtopace!
Generating a bunch files to make one part is error prone imho. I posted a recent project where I made a couple screw less vises. If I had done that project with one g-code file per side per part It would have generated almost 5 times as many files to manage, load and run. The project was done in 4 files for the vise and another dozen for the jaws, stops and accessories. 16 files to manage versus 80 makes a difference to me and I have decent file management and computer skills. This is not including the 16 iges , and 2x cad files totaling 64 files for the project as is. I understand the strategy might be different if I was making 20 at a time and even then I would consider 1 file to complete all parts on all sides with all the fixtures . The setup does become complex in sprut and requires things like 20 stock definitions and maybe 20 part models. There are also more ways to do this with offsets. Sprut allows so many ways to get results its hard to decide what works best.

Add to Jakes comment about export of machine results.
I see this as a cool feature to use over different machines. Start with a part in sbl15, perform operations and export results to stl file that is imported as stock for use in a pcnc mill program. Using this would allow a person to follow results from start to finish across a number of machines. Don't think I can do this in one file hehe

[LRF]

In my application I machine bars of aluminum, 200 of them at a time. Each bar generates 3 completed parts. They are machined in special vise jaws on side 1. I machine all of them and then change the vise jaw setup and drill them on the second side, then flip them and drill the third side. Then I change the setup vise jaws and machine the last fourth side which in the process separates the 3 parts.

If there is a better way of doing the procedure then I will listen. The 4th axis is way to slow to use, too much time is consumed rotating between the axis of the parts. I don't even use my ATC because it is slower then I can change the tools myself. Total tool count change is 19 using 12 unique tools (in other words 7 of the tools get used more then once but of course only once on any given side). I know everyone talks about multitasking while the machine is running, I do also multitask i just need to be at the machine at time of tool change.