Offsetting Letters in the Male Inlay

This forum is for general discussion about Aspire

Offsetting Letters in the Male Inlay

Postby chris77 » Wed Jun 12, 2019 10:13 pm

Hello,

I have cut out some pockets for letters using the Female Inlay Toolpath. When I cut out the letters in the Male Inlay Toolpath the letters were too small. I had tested the fit before hand and it worked good but the only thing different between the two is I used a different kind of wood in the test. I did not know that would make a difference but in this case it did. I tried to change the Allowance Offset in the Male Inlay Settings to make the letters bigger for a snugger fit but I cannot make it work. For example, when I started with 0 allowance then changed it to -.04 and then .04 they both would be the same allowance and they both would be to the inside of the 0 allowance instead of one being inside and the other outside. I tried lots of scenarios but could not make the letters larger. I would appreciate the help!
chris77
 
Posts: 23
Joined: Sun Mar 31, 2019 12:29 pm
Model of CNC Machine: Laguna

Re: Offsetting Letters in the Male Inlay

Postby TReischl » Thu Jun 13, 2019 1:01 am

Offsetting can be problematic, especially when doing small things because you do not notice what is happening.

This may not be good practice. But when I have used the Inlay tool I select a cutter, say .25 dia and I do the male cutout. Then I select the Female section of the Inlay tool and select the same tool. But then I edit the tool diameter using the Edit tool. Typically I will tell it that the tool is .003 or so smaller than it is listed. That causes the pocket to be a bit larger because the software thinks it is using a smaller tool so the tool overcuts a wee bit (as my friend Martin would say).

I do NOT start offsetting vectors because that affects inside corner radii, there is a tutorial floating around about that somewhere, maybe one of the guys who has memorized all the tutorials will wander by and post it.
http://www.tedreischl.com

Low Profile CNC Router Vise
User avatar
TReischl
Vectric Wizard
 
Posts: 2713
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset

Re: Offsetting Letters in the Male Inlay

Postby martin54 » Thu Jun 13, 2019 11:35 am

The allowance offset should work, on a male inlay part the a positive allowance should make the letter bigger & a negative make it smaller. I can never remember which way round allowances go for each type of toolpath so I always set a really large offset & then look at the 2D toolpath view to see how it has cut :lol: :lol:
I have just done that to make sure I posted correct way round above :lol: :lol: :lol:

I always try to cut the male parts first, this way if they are slightly to large then you can increase the allowance a little on the female pocket. Are you using the same vectors & the same tool? Not just the same size tool but actually the same tool? If you are not then that may be part of your problem, Cutting bits are often not exactly the size they claim to be.

It will obviously depend on what size you have overcut the female pocket if the letters are to small, that's another reason for cutting the male letters first, if you cut without any allowance what so ever then the letters are never going to fit in the pockets so normally only a small allowance is required.
0.04 inch is quite large but obviously depends on what sort of fit you are after & what size the letters.

I have just done some Name signs using Oak with 3mm acrylic letters, there were 10 of these in total, the letters are approx 3 inch tall, this was using a 3mm bit with a 0.15mm offset allowance, letters were all a very snug fit :lol: :lol:

path names2.jpg


path names4.jpg
User avatar
martin54
Vectric Wizard
 
Posts: 4526
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Offsetting Letters in the Male Inlay

Postby chris77 » Thu Jun 13, 2019 12:13 pm

That is the problem. When I do a positive or negative allowance offset and look at the 2D toolpath the original 0 toolpath is still the larger offset of the two. Why is that? I cannot figure it out.
chris77
 
Posts: 23
Joined: Sun Mar 31, 2019 12:29 pm
Model of CNC Machine: Laguna

Re: Offsetting Letters in the Male Inlay

Postby martin54 » Thu Jun 13, 2019 1:14 pm

OK now I see what you are saying, just tried again & it doesn't seem to matter what allowance you put on (negative or positive) it cuts the same way.
I always cut the male parts first so when I cut the pocket I am always looking to increase it's size so not encountered this problem with negative or positive ffsets before.

Maybe send an email to Vectric support & ask them if there is a way to do this :lol:

Only way I can think of to do it is to offset your original Vector a very small amount & then use that but as Ted has already said that may cause other problems.
User avatar
martin54
Vectric Wizard
 
Posts: 4526
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Offsetting Letters in the Male Inlay

Postby Adrian » Thu Jun 13, 2019 2:26 pm

It's working the way it's supposed to. The allowances in the inlay toolpahts will reduce the size of a male part and increase the size of a female part. If you need to make the male parts larger then you will have to increase the vector size.

It's explained in the Help for the inlay toolpath.
User avatar
Adrian
Vectric Archimage
 
Posts: 9365
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Offsetting Letters in the Male Inlay

Postby chris77 » Thu Jun 13, 2019 3:21 pm

Ok. Thank you all for the help!
chris77
 
Posts: 23
Joined: Sun Mar 31, 2019 12:29 pm
Model of CNC Machine: Laguna

Re: Offsetting Letters in the Male Inlay

Postby gkas » Thu Jun 13, 2019 10:06 pm

martin54 wrote:The allowance offset should work, on a male inlay part the a positive allowance should make the letter bigger & a negative make it smaller. I can never remember which way round allowances go for each type of toolpath so I always set a really large offset & then look at the 2D toolpath view to see how it has cut :lol: :lol:
I have just done that to make sure I posted correct way round above :lol: :lol: :lol:


....and I thought it was just me that has to check every time I use allowance offset. :?
User avatar
gkas
Vectric Wizard
 
Posts: 392
Joined: Sun Jan 01, 2017 3:39 am
Location: Southern California
Model of CNC Machine: Aspire, Axiom AR8 Pro+, Axiom 4.2W Laser


Return to Aspire - General

Who is online

Users browsing this forum: CEG, Google [Bot], tonydude919 and 28 guests