2 standing problems I am having trouble with

[medaq]

Having trouble getting coolant turned on as default. I am still baffled why defaults or no coolant. But I did  click files from tool path manager, Edit the operation defaults, Select all operations, Edit common, click coolant, and turn it to M08. 

 

The problem I am getting it is defaulting to before. So tool change happens and now it is off. But when editing operation defaults that square is greyed out, so I can not set it to after. 

 

The other issue I am having is optirough stuff. Use a 1/2" endmill. Then a 1/4" with a stock model to clean up everything. But I get a lot of wasted paths. What is some normal settings so the 1/4" is not wasted so much.?I have tried to copy the path and change the tool with the same settings. Then try to add some stock to leave. 

 

 

[jlw™]

Stock model for number 2.  Search the forum, that's been beat to death. 

[Colin Gilchrist]

For setting the "Operation Defaults", you must edit your "Defaults" File, and "Replace" the default Machine Definition, with "your" Machine Definition. Once your "real machine" is set as the Machine Definition inside the Defaults file, you can then go and select each Coolant Option, and set it the way you like it, for each individual Operation Type.

To edit the Defaults File:

1. Make a backup copy of the original file.
2. Change the File Extension of the original Default File to ".mcam". This tells Mastercam the "Defaults" file is just a normal "Mastercam" File. (Which, internally, it is...)
3. Open the Defaults.Mcam file by using File > Open.
4. Replace the MD inside the Machine Group Properties.
5. Edit your Operation Defaults.
6. Save the File.
7. Outside of Mastercam, change the File Extension back to the original.

Happy Programming!

[: Chip :]

You only have two problems?

[Mariana Lendel In-House Solutions]

The second issue. I am guessing, in the OptiRough, you are using the Stock dialog box and enabled Rest material.

I will go with Compute remaining stock from One other operation and select the OptiRough with the 1/2" tool.

Adjustments to remaining stock can be set to Ignore small cusps and you can leave the distance to 0 or add a small amount.

If you want the tool to retract and machine the corners, in the Cut parameters you should set the Motion > Gap size retract to.

Enable  When exceeding a distance or/and  Avoiding a boundary and set the distance as needed based on your model. Otherwise Mastercam  keeps the tool down.

I would set Linking to Full Vertical Retract and the Linear entry/exit to a bigger value.  You will get a lot of rapid moves unfortunately.

 

[: Chip :]

I too have issues with Opti-Rough. I like the HSS features but a lot of the issues I have a difficult time controlling the feature based parameters. 

Sometimes this doesn't achieve the depths I'm trying for but multi contours/pockets/profiles, matl removal is bitchen.

I find my self extracting what Opti-Rough gives me and Dynamic Contouring what I don't get. 

Dynamic Countour is cool for 2018. (I have yet to make a Tool path in 2018 but I like the chaining updates) the chaining once you get use to it can make your path super fast and efficient. 

 

You'd be surprised, the tineyist piece of matl. Draw a profile and Dynamic that corner out as fast as your machine'll go.

For me Hybrid Roughing is just that. Matl removal something YOU CAN REALLY TRUST a "go to Tool path" to stay within a boundary and not gouge your project

:CHIP:

[sophiaedward64]

Strongly agree with Colin. 

[zachlancy]

For machining rest material I turn the precision to max in verify, save the outcome as an stl somewhere, then use that in the optirough stock page as my "stock". Use CAD File and point it to the .stl. Not sure if the verify precision has any impact on the accuracy of the stl, but i figure it cant hurt. Usually works alright for me.

[nickbe10]

On 7/19/2017 at 6:59 PM, medaq said:

The other issue I am having is optirough stuff. Use a 1/2" endmill. Then a 1/4" with a stock model to clean up everything. But I get a lot of wasted paths. What is some normal settings so the 1/4" is not wasted so much.?I have tried to copy the path and change the tool with the same settings. Then try to add some stock to leave. 

I save an .stl and use that as my rest material source. Seems to work well. It recognizes slopes and geometry which clearly are affecting the toolpath .

[crazy^millman]

10 hours ago, zachlancy said:

For machining rest material I turn the precision to max in verify, save the outcome as an stl somewhere, then use that in the optirough stock page as my "stock". Use CAD File and point it to the .stl. Not sure if the verify precision has any impact on the accuracy of the stl, but i figure it cant hurt. Usually works alright for me.

Not a good way to do it if you share files across a network or send files offsite to customers to run them. The link gets broken and the files becomes unusable. Keep everything in the file and when the file gets to large you then break up the file per operations to keep stability.

[Colin Gilchrist]

10 hours ago, zachlancy said:

For machining rest material I turn the precision to max in verify, save the outcome as an stl somewhere, then use that in the optirough stock page as my "stock". Use CAD File and point it to the .stl. Not sure if the verify precision has any impact on the accuracy of the stl, but i figure it cant hurt. Usually works alright for me.

I agree with Ron on the issue of linking to an "external STL file". This can break your Mastercam file, if you share files across the network, and something gets moved.

The better solution is simply to add a quick extra step.

Once you have "output" your STL from Verify, use File > Merge, to bring in the STL File as a "Pmesh" entity into Mastercam.

When you pull up the "Merge File" dialog (just says "Open" as the title), change the "File Type" to "StereoLithography Files (*.stl). When you do this, an "Options" button appears. Click it.

In the STL Read Parameters dialog, you can choose between "Mesh" and "Lines", but, you can also use the "Stitch Triangles" function to reduce the amount of data in the Pmesh file, by filtering out the small triangles. A filter does always change the resolution of the curved surfaces, but shouldn't change the actual dimensional accuracy of the "flat areas" much. Try importing the Pmesh file, 5 times - on 5 different levels, with the following "Stitch Tolerances":

Try the following Stitch Tolerances, while importing another (new) Pmesh. Be sure to change levels between imports:

1. 0.002
2. 0.004
3. 0.010
4. 0.020
5. 0.040

I've seen some really big STL files get reduced considerably, without really changing the true envelope of the STL "surfaces" that much. I say "surfaces" in quotes, because the STL itself is simply a collection of Trianglular facets, with a normal direction.

Now, when you create a Stock Model, you can link it to one of the Pmesh Entities, which is now stored inside your Mastercam File. This means the "link" won't get broken in the Stock Model, and more importantly, there is very little "calculation time" when generating the Stock Model, because all it really has to do is display the already "Stitched" Pmesh entity. You will also find your Toolpath that reference a Stock Model will now calculate faster, as the amount of data (triangle count, and triangle size) has been enhanced. (less triangles, and the remaining triangles are bigger.)