Simple two operation part

[honk]

Hi every one just a question on best method for this simple procedure.

I have a part that im turning in the lathe simple part.

OP1 face and turn partial od.
OP2 face rough profile finish.

Now what the best way to do this in Edgecam.

I want the program so when op1 is finished i get m00 flip the part around and hit start again.

Do i write two separate programs and join them bring in two models and rotate one. I would like the simulation to look correct as well.

Thanks.

I find with Edgecam the simple stuff is the stuff it does very bad. What should be easy never is.

[jstikeleather]

Hello,
So what you want to do is the following:

OP1: face and rough turn OD
Flip the part around
OP2: face and rough turn OD then finish profile

You have a couple options:
1. Use two part files, one for standard orientation, one for reverse orientation
2. Use one part file but have two sequences

Using the first option should be pretty straight forward. Output the code for both programs and then use copy/paste to get it into one file.

The second option you will need to create a second CPL on the origin of the back of the part. When you are in the manufacturing side and select "file > new sequence" it will prompt you for the initial CPL, this would be the CPL you had made on the back face.

Make sure that Z is pointing in the correct direction.

Then program it accordingly. You will still have to output two programs and then copy/paste them together.

The convenience of option 2 is that you only have one PPF file and when you simulate it will look correct. For option 1 to simulate correctly you will have to save the stock model as an STL and import it into the second file.

Good luck.
Jeremiah Stikeleather
ATS

[honk]

Thanks i had programmed it using method two method one does not work for fixture checking as the part is held in a chuck. It looks like your machining through the chuck all the time.

You would think such a common practice in lathe turning would be easy, and have the option in Edgecam so it simulates correct and you dont need to mess with pasting programs and stuff.

Thanks for the input.

[inflateable]

I do it Jerimiah's second way, but then I don't show the chuck on screen.
In simulator just turn the machine off, (so you can only see the part, floating in midair)and it'll look fine.

Simulating the machine for a lathe just isn't worth the hassle.

[honk]

Originally Posted by jstikeleather Hello, So what you want to do is the following: OP1: face and rough turn OD Flip the part around OP2: face and rough turn OD then finish profile You have a couple options: 1. Use two part files, one for standard orientation, one for reverse orientation 2. Use one part file but have two sequences Using the first option should be pretty straight forward. Output the code for both programs and then use copy/paste to get it into one file. The second option you will need to create a second CPL on the origin of the back of the part. When you are in the manufacturing side and select "file > new sequence" it will prompt you for the initial CPL, this would be the CPL you had made on the back face. Make sure that Z is pointing in the correct direction. Then program it accordingly. You will still have to output two programs and then copy/paste them together. The convenience of option 2 is that you only have one PPF file and when you simulate it will look correct. For option 1 to simulate correctly you will have to save the stock model as an STL and import it into the second file. Good luck. Jeremiah Stikeleather ATS

I tried the second option just to see what would happen, i could not describe a CPL that had only two axis it kept given me 3 axis.
Also when typing in X positions it is no longer working in Diameter, and the tool is the wrong way, well the correct way but obviously if im trying to machine the back of the part and trick Edgecam into thinking its the front the right hand tool should be the other way.

So are you saying i also need to select a lefthand tool and change the name to right

Thanks

[jstikeleather]

Originally Posted by honk I tried the second option just to see what would happen, i could not describe a CPL that had only two axis it kept given me 3 axis.

Look at your options when creating a CPL. You may just want to create a CPL referenced from the Turn CPL, then rotate it 180 around X.

Originally Posted by honk Also when typing in X positions it is no longer working in Diameter, and the tool is the wrong way, well the correct way but obviously if im trying to machine the back of the part and trick Edgecam into thinking its the front the right hand tool should be the other way. So are you saying i also need to select a lefthand tool and change the name to right Thanks

Those X values being radial are more than likely because of the 3rd axis on the CPL you made.

If you created a new sequence and defined your new initial CPL to be the CPL you created (which is just the reverse of the original Turn CPL) then your tools will be pointed in the correct direction. You are more than likely not defining a new sequence, or you are not correctly defining the initial CPL.

[honk]

Originally Posted by jstikeleather Look at your options when creating a CPL. You may just want to create a CPL referenced from the Turn CPL, then rotate it 180 around X. Those X values being radial are more than likely because of the 3rd axis on the CPL you made. If you created a new sequence and defined your new initial CPL to be the CPL you created (which is just the reverse of the original Turn CPL) then your tools will be pointed in the correct direction. You are more than likely not defining a new sequence, or you are not correctly defining the initial CPL.

I think its the CPL thats getting defined wrong but i cannot see any options anywhere to change that. Scrap that just noticed when creating a CPL there is a box to change if its a mill or lathe CPL.

Thanks for the input

[jsanders]

Originally Posted by honk Thanks i had programmed it using method two method one does not work for fixture checking as the part is held in a chuck. It looks like your machining through the chuck all the time. You would think such a common practice in lathe turning would be easy, and have the option in Edgecam so it simulates correct and you dont need to mess with pasting programs and stuff. Thanks for the input.

Remember to also contact your reseller and have them log a development request on behalf of YOUR COMPANY to support part flip. Edgecam development is prioritized based on frequency of request, so your reseller needs to carry through with making a formal request. You can ask your reseller to let you know what the case # is so that you can pester them to get an update.

If everyone assumes that someone else is making a request, then no one is.

[honk]

Can some one elaborate a bit more on this i thought i had it tried again just now and 2nd way does not work for me always give a 3axis CPL and then will not do anything, and wont go the correct direction im obviously missing something but cant see what.

Thanks

[jstikeleather]

Originally Posted by honk Can some one elaborate a bit more on this i thought i had it tried again just now and 2nd way does not work for me always give a 3axis CPL and then will not do anything, and wont go the correct direction im obviously missing something but cant see what. Thanks

How are you creating your "back end" cpl?

Try the following:
1. On the Design side and from the menu, click Geometry > Create CPL.
2. Click on the Reference tab, select Inv Turn.
3. Click on the General tab, check the Origin box, specify a name, check your Work Plane and Dimensions.
4. Select the new location of your CPL (select the back end of the part).

If you have trouble placing the CPL in the correct location, use Coordinate Input.

When you create your new sequence, select this new CPL as your Initial CPL.